Lusas Example Manual

Transcript

Examples Manual LUSAS Version 14 : Issue 2 LUSAS Forge House, 66 High Street, Kingston upon Thames, Surrey, KT1 1HN, United Kingdom Tel: +44 (0)20 8541 1999 Fax +44 (0)20 8549 9399 Email: [email protected] http://www.lusas.com Distributors Worldwide Table of Contents Table of Contents Introduction 1 Where do I start?..................................................................................................................... 1 About the examples ................................................................................................................ 1 Format of the examples.......................................................................................................... 2 Running LUSAS Modeller....................................................................................................... 5 Creating a new model / Opening an existing model ............................................................ 6 Creating a Model from the Supplied VBS Files .................................................................... 7 The LUSAS Modeller Interface ............................................................................................... 8 Linear Elastic Analysis of a Spanner 11 Description ............................................................................................................................ 11 Modelling : Features ............................................................................................................. 12 Modelling : Attributes ........................................................................................................... 21 Running the Analysis............................................................................................................ 32 Viewing the Results .............................................................................................................. 33 Calculating Section Properties of a Box Section 45 Description ............................................................................................................................ 45 Modelling ............................................................................................................................... 46 Nonlinear Analysis of a Concrete Beam 51 Description ............................................................................................................................ 51 Modelling ............................................................................................................................... 52 Running the Analysis............................................................................................................ 63 Viewing the Results .............................................................................................................. 64 Contact Analysis of a Lug 71 Description : Linear Material................................................................................................ 71 Modelling : Linear Material................................................................................................... 72 Running the Analysis : Linear Material ............................................................................... 79 Viewing the Results : Linear Material.................................................................................. 80 Description : Nonlinear Material .......................................................................................... 86 Modelling : Nonlinear Material ............................................................................................. 86 Running the Analysis : Nonlinear Material ......................................................................... 94 Viewing the Results : Nonlinear Material............................................................................ 95 Linear Buckling Analysis of a Flat Plate 103 Description .......................................................................................................................... 103 Modelling ............................................................................................................................. 104 Running the Analysis.......................................................................................................... 109 Viewing the Results ............................................................................................................ 110 Elasto-Plastic Analysis of a V-Notch 113 Description .......................................................................................................................... 113 Modelling : Linear Material................................................................................................. 115 Running the Analysis : Linear Material ............................................................................. 121 Viewing the Results : Linear Material................................................................................ 122 Modelling : Nonlinear Material ........................................................................................... 124 Running the Analysis : Nonlinear Material ....................................................................... 127 Viewing the Results : Nonlinear Material.......................................................................... 129 Modelling : Contact Analysis (Linear Material)................................................................. 132 Running the Analysis : Contact Analysis (Linear Material)............................................. 138 Viewing the Results - Contact Analysis (Linear Material) ............................................... 140 Modelling : Contact Analysis (Nonlinear Material)........................................................... 141 Running the Analysis : Contact Analysis (Nonlinear Material) ....................................... 143 i Introduction Viewing the Results : Contact Analysis (Nonlinear Material)..........................................144 Modal Analysis of a Tuning Fork 149 Description...........................................................................................................................149 Modelling..............................................................................................................................150 Running the Analysis ..........................................................................................................162 Viewing the Results.............................................................................................................163 Modal Response of a Sensor Casing 173 Description...........................................................................................................................173 Modelling..............................................................................................................................174 Running the Analysis ..........................................................................................................181 Viewing the Results.............................................................................................................183 Thermal Analysis of a Pipe 193 Description...........................................................................................................................193 Modelling..............................................................................................................................194 Running the Analysis ..........................................................................................................198 Viewing the Results.............................................................................................................200 Transient Thermal Analysis................................................................................................201 Running the Analysis ..........................................................................................................204 Viewing the Results.............................................................................................................204 Linear Analysis of a Composite Strip 207 Description...........................................................................................................................207 Modelling : Shell Model.......................................................................................................208 Running the Analysis ..........................................................................................................220 Viewing the Results.............................................................................................................221 Modelling : Solid Model ......................................................................................................223 Running the Analysis ..........................................................................................................227 Viewing the Results.............................................................................................................229 Damage Analysis of a Composite Plate 233 Description...........................................................................................................................233 Modelling..............................................................................................................................234 Running the Analysis ..........................................................................................................243 Viewing the Results.............................................................................................................245 Mixed-Mode Delamination 247 Description...........................................................................................................................247 Modelling : Delamination Model.........................................................................................248 Running the Analysis ..........................................................................................................260 Viewing the Results.............................................................................................................261 ii Where do I start? Introduction Where do I start? Start by reading this introduction in its entirety. It contains useful general information about the Modeller User Interface and details of how the examples are formatted. The first example in this manual contains detailed information to guide you through the procedures involved in building a LUSAS model, running an analysis and viewing the results. This fully worked example details the contents of each dialog used and the necessary text entry and mouse clicks involved. The remaining examples assume that you have completed the fully worked example and may not necessarily contain the same level of information. The examples are of varying complexity and cover different modelling and analysis procedures using LUSAS. It will benefit you to work through as many as possible, even if they have no direct bearing on your immediate analysis interests. About the examples Unless otherwise noted, the examples are written for use with the base versions of all LUSAS V14 software products. The LUSAS software product and any product options that are required will be stated at the beginning of the example. Except where mentioned, all examples are written to allow modelling and analysis to be carried out with the Teaching and Training version of LUSAS which has restrictions on problem size. The limits are currently set as follows: 500 Nodes 100 Points 250 Elements 1500 Degrees of Freedom 10 Loadcases Because of the modelling and analysis limits imposed by the Teaching and Training Versions some examples may contain coarse mesh arrangements that do not necessarily constitute good modelling practice. In these situations these examples should only be used to illustrate the LUSAS modelling methods and analysis procedures involved and should not necessarily be used as examples of how to analyse a particular type of structure in detail. 1 Introduction Format of the examples Headings Each example contains some or all of the following main headings: Description contains a summary of the example, defining geometry, material properties, analysis requirements and results processing requirements. • Objectives states the aims of the analysis. • Keywords contains a list of keywords as an aid to selecting the correct examples to run. • Associated Files contains a list of files held in the \\Examples\Modeller directory that are associated with the example. These files are used to re-build models if you have problems, or can be used to quickly build a model to skip to a certain part of an example, for instance, if you are only interested in the results processing stage. Modelling contains procedures for defining the features and attribute datasets to prepare the LUSAS model file. Multiple model files are created in some of the more complex examples and these therefore contain more than one ‘Modelling’ section. Running the Analysis contains details for running the analysis and assistance should the analysis fails for any reason. Viewing the Results contains procedures for results processing using various methods. Menu commands Menu entries to be selected are shown as follows: Geometry Point Coordinates... > This implies that the Geometry menu should be selected from the menu bar, followed by Point, followed by the Coordinates... option. Sometimes when a menu entry is referred to in the body text of an example it is written using a bold text style. For example the menu entry shown above would be written as Geometry > Point > Coordinates... 2 Format of the examples Toolbar buttons For certain commands a toolbar button will also be shown to show the ‘short-cut’ option to the same command that could be used instead: The toolbar button for the Geometry > Point > Coordinates… command is shown here. User actions Actions that you need to carry out are generally bulleted (the exception is when they are immediately to the right of a menu command or a toolbar button) and any text that has to be entered is written in a bold text style as follows: • Enter coordinates of (10, 20). So the selection of a typical menu command (or the equivalent toolbar button) and the subsequent action to be carried out would appear as follows: Geometry Point Coordinates... > Enter coordinates of (10, 20). Selecting the menu commands, or the toolbar button shown will cause a dialog box to be displayed in which the coordinates 10, 20 should be entered. Filling-in dialogs For filling-in dialogs a bold text style is used to indicate the text that must be entered. Items to be selected from drop-down lists or radio buttons that need to be picked also use a bold text style. For example: • In the New Model dialog enter the filename as example. • In the Model details section enter the model title as Test component. Set the Startup template as Standard. Ensure the Vertical axis is set to Z • Click the OK button to finish. 3 Introduction Grey-boxed text Grey-boxed text indicates a procedure that only needs to be performed if problems occur with the modelling or analysis of the example. An example follows: Rebuilding a model File New… Start a new model file. If an existing model is open Modeller will prompt for unsaved data to be saved before opening the new file. • Enter the file name as example File Script Run Script... > To recreate the model, select the file example_modelling.vbs located in the \\Examples\Modeller directory. Visual Basic Scripts Each example has an associated set of LUSAS-created VBS files that are supplied on the release kit. These are installed into the \\Examples\Modeller directory. These scripts are for use when it proves impossible for you to correct any errors made prior to running an analysis. They allow you to re-create a model from scratch and run an analysis successfully Modelling Units At the beginning of each example the modelling units used will be stated something like this: “Units used are N, m, kg, s, C throughout” Care must be taken to ensure that in real-life modelling situations consistent modelling units are used. In particular, in analyses where the self weight of the structure is to be considered, adjustment must be made to the Young’s Modulus and Mass Density material property values to ensure that the correct output results are obtained. Icons Used Throughout the examples, files, notes, tips and warnings icons will be found. They can be seen in the left margin. Files. The diskette icon is used to indicate files used or created in an example. 4 Running LUSAS Modeller Note. A note is information relevant to the current topic that should be drawn to your attention. Notes may cover useful additional information or bring out points requiring additional care in their execution. Tip. A tip is a useful point or technique that will help to make the software easier to use. Caution. A caution is used to alert you to something that could cause an inadvertent error to be made, or a potential corruption of data, or perhaps give you results that you would not otherwise expect. Cautions are rare, so take heed if they appear in the example. Running LUSAS Modeller • Start LUSAS Modeller from the start programs menu. Typically this is done by selecting: Start > All Programs > LUSAS 14.x for Windows > LUSAS Modeller • The on-line help system will be displayed showing the latest changes to the software. • Close the on-line Help system window. (LUSAS Academic version only) • Select your chosen LUSAS product and click the OK button. 5 Introduction Creating a new model / Opening an existing model When running LUSAS for the first time the LUSAS Modeller Startup dialog will be displayed. This dialog allows either a new model to be created, or an existing model to be opened. Note. When an existing model is loaded a check is made by LUSAS to see if a results file of the same name exists. If so, you have the option to load the results file on top of the opened model. Note. When an existing model is loaded, that in a previous session crashed forcing LUSAS to create a recovery file, you have the option to run the recovery file for this model and recover your model data. 6 Creating a Model from the Supplied VBS Files If creating a new model the New Model dialog will be displayed. • Enter information for the new model information and click the OK button. Product specific menu entries for the selected software product in use e.g. Analyst, Composite, Bridge or Civil will be added to the LUSAS Modeller menu bar. Creating a Model from the Supplied VBS Files If results processing and not the actual modelling of an example is only of interest to you the VBS files provided will allow you to quickly build a model for analysis. Proceed as follows to create the model from the relevant VBS file supplied: File New… Start a new model file. • File Script Run Script... > Enter the file name as example name and click OK Select the file example_name_modelling.vbs located in the \\Examples\Modeller directory. Note. VBS scripts that create models automatically perform a File > Save menu command. 7 Introduction The LUSAS Modeller Interface Modelling in LUSAS A LUSAS model is graphically represented by geometry features (points, lines, surfaces, volumes) which are assigned attributes (mesh, geometric, material, support, loading etc.). Geometry is defined using a whole range of tools under the Geometry menu, or the buttons on the Toolbars. Attributes are defined from the Attributes menu. Once defined attributes are listed in the Treeview. Treeview Treeviews are used to organise various aspects of the model in graphical frames. There are a number of Treeviews showing Layers , Groups , Attributes , Loadcases , Utilities , and Reports . Treeviews use drag and drop functionality. For example, an attribute in the Treeview can be assigned to model geometry by dragging the attribute onto an object (or objects) currently selected in the graphics window, or by copying and pasting an attribute onto another valid Treeview. Treeview item as for instance, a group name, as held in the groups 8 The LUSAS Modeller Interface Context Menus Although commands can be accessed from the main menu, pressing the right-hand mouse button with an object selected usually displays a context menu which provides access to relevant operations. Getting Help LUSAS contains a comprehensive Help system. The Help consists of the following: on the Main toolbar is used to get context-sensitive help on • The Help button the LUSAS interface. Click on the Help button, then click on any toolbar button or menu entry (even when greyed out). • Every dialog includes a Help button which provides information on that dialog. • Selecting Help > Help Topics from the main menu provides access to all the Help files. After a help page is first displayed pressing the Show button will provide access the full Help Contents, the Help Index and the Search facility. 9 10 Description Linear Elastic Analysis of a Spanner For software product(s): With product option(s): All. None. Description A linear static analysis is to be carried out on the spanner shown. The spanner is supported as though it were being used to turn a nut, and is loaded with a constant pressure load along the top edge of the handle. 20 20 10 Spline Line defined as a tangent to an arc and a construction Line 40 20 40 160 Units used are N, mm, t, s, C, throughout. Keywords 2D, Linear, Elastic, Regular Meshing, Irregular Meshing, Copy, Rotate, Mirror, Transformation, Groups, Deformed Shape, Contour Plot, Principal Stress Vector Plot, Graph Plotting, Slice Section Results. 11 Linear Elastic Analysis of a Spanner Objectives The required output from the analysis is: A plot of the deformed shape. A plot of the equivalent stresses in the spanner. A graph showing the variation in equivalent stress where the handle meets the jaws. Associated Files spanner_modelling.vbs carries out the modelling of the example. Modelling : Features This section covers the definition of the features (Points, Lines and Surfaces) which together form the geometry of the spanner. The symmetry of the spanner will be used by firstly defining one half and then mirroring about a horizontal centre-line. One half of the jaws will be defined by three Surfaces using 3 different methods. One Surface will be defined simply by its bounding coordinates, a second by sweeping a Line through a rotational transformation and a third by copying the second Surface using a pre-defined rotation. One half of the handle will be defined using one Surface. It will be bounded by three Lines, one of which will be a cubic spline. Once the Surfaces have been defined, they will all be mirrored about the spanner centre-line. The features which make up the spanner will be divided into two Groups, the jaws and the handle, to make the assignment of attributes easier. Running LUSAS Modeller For details of how to run LUSAS Modeller see the heading Running LUSAS Modeller in the Examples Manual Introduction. Note. This example is written assuming a new LUSAS Modeller session has been started. If continuing from an existing Modeller session select the menu command File>New to start a new model file. Modeller will prompt for any unsaved data and display the New Model dialog. 12 Modelling : Features Creating a new model • Enter the file name as spanner • Use the Default working folder. • Enter the Spanner title as the units • Set N,mm,t,s,C as the model • Select template Standard from those available in the drop down list. • Leave the user interface set to Structural • Ensure the Vertical Axis is set to Z • Click the OK button. Note. Save the model as the example progresses. The Undo button may be used to correct a mistake. The undo button allows any number of actions since the last save to be undone. Modelling Geometry LUSAS Modeller is a feature-based modelling system. The model geometry is defined in terms of features (Points, Lines, Surfaces and Volumes) which are later meshed to generate the Finite Element Model ready for solution. The features form a hierarchy, with Points defining Lines, Lines defining Surfaces and Surfaces defining Volumes. 13 Linear Elastic Analysis of a Spanner Geometry Surface Coordinates... > Enter coordinates of (0, 20), (-20, 20), (-20, 30) and (0, 40) to define the vertices of the Surface. Note. Sets of coordinates are separated by commas or spaces. The Tab key is used to create new entry fields. The arrow keys are used to move between entries. • Click the OK button to make the dialog disappear and generate the Surface as shown. Note. If the Z ordinate is omitted zero is assumed. Note. Confirmation that the Surface has been created is given in the message window. Note. Cartesian, cylindrical or spherical coordinates systems may be used to define models. In this example Cartesian coordinates will be used throughout. The right-hand vertical Line will be used to create a Surface by sweeping the line through a rotation of 45 degrees clockwise. • Select the Line by moving the cursor over the Line shown and clicking the left-hand mouse button. Select this Line The line will change colour to show it has been selected. Note. Feedback on the items currently selected is provided on the right-hand side of the status bar at the bottom of the display. ... and sweep it to form this Surface 14 Modelling : Features Geometry Surface By Sweeping.. > Select the Rotate option and enter -45 for the angle of rotation about the Z-axis. • Enter the attribute name as Rotate 45 Clockwise • Click the Save button to save the dataset for re-use later. • Click the OK button to sweep the Line clockwise through 45 degrees about (0,0,0) to create a Surface. Note. Clockwise angles are negative and anti-clockwise angles are positive. The Surface just drawn will now be copied by rotating it through a 45 degree rotation clockwise. • Select the previously drawn Surface by clicking on it with the left-hand mouse button. Select and copy this Surface To form this Surface 15 Linear Elastic Analysis of a Spanner Geometry Surface Copy... > Select the attribute Rotate 45 Clockwise from the drop down list. • Ensure that the number of copies is set to 1 • Click the OK button to copy the Surface, rotating it clockwise through 45 degrees. To define the top line of the handle of the spanner a cubic spline will be created. Note. A cubic spline is a Line which passes through any number of Points. If required, the start and finish directions of the spline can be defined by specifying endtangents (i.e. by specifying the directions of Lines at its ends). In this example end-tangents are used to fix the start and finish directions of the spline so a construction Line must first be defined. Geometry Line Coordinates... > Enter coordinates of (200, 0) and (200, 10) to define the construction Line. • Click the OK button to generate a vertical Line away from the existing Surfaces. This Line will be used to specify the finishing direction of the cubic spline. Note. When selecting features to define a cubic spline it is very important that the correct features are selected in a particular order. The Lines that define the start and finish directions of the spline are to be selected first, followed by the Points that define the start and end positions of the spline. 16 Modelling : Features Defining a cubic spline • Select the arc shown by moving the mouse over the arc and click the left-hand mouse button. (This arc defines the direction in which the spline starts). 1. Select this arc 3. Select this Point 4. Select this Point • Hold the Shift key down to add additional features to the selection 2. Select this Line • Select the construction Line defined earlier by moving the mouse over the Line shown and click the left-hand mouse button. (This Line defines the direction in which the spline ends). • Continue holding the Shift key down to further add to the selection. Select the Point on the end of the first arc selected. (This defines where the spline starts). • Still holding the Shift key down, select the Point on the end of the construction Line. (This defines where the spline ends). Geometry Line Spline Tangent to Lines... Generates a cubic spline to form the handle of the spanner. > > Once the spline is drawn correctly the construction Line is deleted. • Drag a box around the construction Line by firstly moving the mouse above and to the left of the Line. Drag a box around the construction Line • Click the left-hand mouse button and holding it down move the mouse to the right and down so that a box is shown which completely encloses the Line as shown. Release the left-hand mouse button. LUSAS will highlight the selected features. Edit Delete Delete the selected features. • Click the Yes button to delete the Lines 17 Linear Elastic Analysis of a Spanner • Click the Yes button again to delete the Points. The centre-line of the spanner can now be defined by joining the two unconnected points into a Line. • Drag a box around the two Points on the centre-line of the spanner as shown Drag a box around these 2 Points Geometry Line Points... > A Line will be drawn between the points selected. The Surface forming the handle of the spanner will now be defined by selecting the three Lines bounding the Surface. • Select the 3 Lines which define the Surface of the handle in the order shown, ensuring the Shift key is held down to keep adding to the selection. Geometry Surface Lines... > 1. Select this Line 2. Hold Shift key down 3. With Shift key down select this Line 4. With Shift key down select this Line To draw the Surface formed by the 3 lines selected. Note. Selecting the Lines in this anti-clockwise order ensures that the local element axes of the Surface will be suitable for the applied face loading that will be applied later in the example. Selecting the Lines by dragging a box around them would not necessarily produce the same Surface axes. Mirroring model information Half of the model has now been defined. This half can now be mirrored to create the whole model. The first step in the process is to define a mirror plane. 18 Modelling : Features • Select the 2 points shown, making sure the Shift key is held down in order to add the second Point to the initial selection. 1. Select this Point 2. Hold the Shift key down These Points define the axis about which the spanner will be mirrored. Edit Selection Memory > Set 3. Select this Point Places the Points selected into memory. Next, the Surfaces to be mirrored are to be selected. This will require the whole model to be selected. Note. An alternative to dragging a box around all the features to select them is to press the Ctrl and A keys at the same time. • Select the whole model by dragging a box around the features or by using the keyboard shortcut described previously. Geometry Surface Copy… > Select Mirror – from Point 14 and Point 15 from the drop down list and click the Use button on the dialog to use the points previously stored in memory. • Click the OK button to copy all of the Surfaces, mirroring them about the centre-line to give the model shown in the previous diagram. If the model features have been mirrored successfully the Points held in memory may be cleared. Edit Selection Memory > Clear The Points are now cleared from memory. This has completed the spanner geometry. 19 Linear Elastic Analysis of a Spanner Using Groups Tip. Model features can be grouped together to make assignment and viewing of model attributes easier. In this example the Surfaces defining the jaws of the spanner will form one Group. The Surfaces defining the handle of the spanner will form another Group. • Drag a box around the Surfaces representing the jaws of the spanner. Geometry Group New Group > Adds a New Group entry to the Treeview for the features selected. Drag a box to select the Jaw features • Enter the group name as Jaws and click OK to finish defining the group. • Drag a box around the Surfaces representing the handle of the spanner. Geometry Group New Group > Adds a New Group entry to the Treeview for the features selected. Drag a box to select the Handle features • Enter the group name as Handle and click OK to finish defining the group. Modelling Features Recap The features that form the 2-Dimensional representation of the spanner have been defined. In this section the following topics have been covered: How to define Points, Lines and Surfaces. How to define Lines by specifying the coordinates of their Points and by joining existing Points. 20 Modelling : Attributes How to define Surfaces by their bounding coordinates, by sweeping, and by copying. How to define a cubic spline. How to select features by using the Shift Key to add to a previous selection. How to select features by dragging a box around features to be selected. How to select all features in a model by pressing the Control and A keys. How to rotate and mirror model features. How to define groups of features. Modelling : Attributes Defining and Assigning Model Attributes In order to carry out an analysis of the model various attributes must be defined and assigned to the model. The following attributes need to be defined: The finite element mesh to be used. The thickness of the spanner. The material from which the spanner is made. The supports to be used. The loading on the spanner. 21 Linear Elastic Analysis of a Spanner Note. LUSAS Modeller works on a define and assign basis where attributes are first defined, then assigned to features of the model. This can be done either in a step-by-step fashion for each attribute or by defining all attributes first and then assigning all in turn to the model. Attributes are first defined and are subsequently displayed in the Treeview as shown. Unassigned attributes appear ‘greyed-out’. Attributes are then assigned to features by dragging an attribute dataset from the Treeview onto previously selected features. Tip. Useful commands relating to the manipulation of attributes can be accessed by Treeview, then selecting an attribute in the clicking the right-hand mouse button to display a shortcut menu. Defining the Mesh The spanner will be meshed using both regular and irregular Surface meshes. A regular mesh is to be used for the jaws of the spanner. An irregular mesh will be used for the handle. The number of elements in the regular Surface mesh will be controlled by defining line meshes on the Lines defining the boundary of the Surfaces. The number of elements in the irregular Surface mesh will be controlled by specifying an ideal element size. Other methods of controlling mesh density are also available. 22 Modelling : Attributes Defining a regular Surface mesh Attributes Mesh Surface… > • Select Plane stress elements, which are Quadrilateral in shape with a Quadratic interpolation order. • Ensure that the Regular Mesh button is selected. • Enter the attribute name as Regular Plane Stress • Click the OK button to add the Surface mesh dataset to the Treeview. The mesh will be assigned to the model at a later stage. Controlling mesh density The lines currently defined have 4 divisions per line by default, but in this example only 2 divisions are required for the Lines defining the jaws. This can be done by either changing the default number of divisions per Line or by making use of Line mesh attributes. In this example, the default number of divisions will be changed. File Model Properties… • Select the Meshing tab and set the Default Line divisions to 2. • Click the OK button. 23 Linear Elastic Analysis of a Spanner Defining an irregular Surface mesh Attributes Mesh Surface… > • Select Plane stress, Triangle, Quadratic elements. • Select Irregular button. the mesh • Enter a Specified element size of 18 • Enter the attribute name as Irregular Plane Stress. • Click the OK button to add the Surface mesh attribute to the Treeview. The mesh will be assigned to the model at a later stage. Defining the Thickness So far the spanner has been defined in two dimensions. In order to give the spanner its thickness geometry attributes will be used. The jaws of the spanner are 15mm thick whilst the handle is 10mm thick. Two geometry attributes are required. Attributes Geometric Surface… > • Enter the thickness as 15. • Enter the Attribute name as Thickness=15 • Click the Apply button to add the geometry attribute Treeview. to the 24 Modelling : Attributes Note. The Apply button allows information for another attributes to be entered using the same dialog. • Change the thickness to 10 • Change the attribute name to Thickness=10 and click the OK button to add the additional geometry attribute to the Treeview. Assigning a Surface mesh and Thickness to the Jaws The Surface mesh and geometry attributes defined previously can now be assigned to the relevant features of the spanner. As an alternative to selecting features by dragging a box around them, named Groups can be used. Treeview click the right-hand mouse button on the group name Jaws • In the and select the Select Members option from the menu. If you already have some features selected click Yes to deselect them first. • Drag and drop the Surface mesh attribute Regular Plane Treeview Stress from the onto the selected Surfaces. Modeller will confirm the mesh assignment for each Surface in the text window. The element mesh for the jaws of the spanner will be drawn. • Drag and drop the Surface geometry attribute Thickness=15 from the Treeview onto the selected Surfaces. The elements of the jaws remain selected. • Click the left-hand mouse button in a blank part of the Graphics Window to deselect any previously selected model features. This shows that the geometric assignment has been visualised by default. Select the fleshing on/off button to turn-off geometric property visualisation. Assigning Surface mesh and Thickness to the Handle • Click the right-hand mouse button on the Group name Handle and select the Select Members option from the menu. All Surfaces forming the group Handle will be selected. 25 Linear Elastic Analysis of a Spanner • Drag and drop the Surface mesh attribute Irregular Plane Stress from the Treeview onto the selected Surfaces defining the Handle. LUSAS will draw the irregular element mesh for the handle of the spanner. Note. The text output window will show messages relating to the radius of curvature for two of the elements created. These can be ignore for this example. • Drag and drop the Surface geometry attribute Thickness=10 from the Treeview onto the selected Surfaces. Again confirmation of the assignment is provided in the text window. • Click the left-hand mouse button in a blank part of the Graphics Window to deselect any previously selected model features. Defining the Material Attributes Material > Material Library… • Select the material Mild Steel from the drop down list, select units of N,mm,t,s,C and click OK to add the material attribute Treeview. to the • With the whole model selected (Ctrl and A keys together) drag and drop the material attribute Steel Ungraded Mild (N,mm,t,s,C) from the Treeview onto the selected features and assign to the selected surfaces by clicking the OK button. 26 Modelling : Attributes Visualising Model Attributes Note. Any attributes (i.e. geometry, material, supports etc.) assigned to the model can be checked visually to ensure that the correct item has been assigned to the correct part of the model. For example: • Click the left-hand mouse button in a blank part of the Graphics Window to deselect any previously selected model features. Treeview, click the right-hand mouse button on the Thickness=15 • In the material attribute name and select the Visualise Assignments option from the dialog. All features to which the Thickness=15 attribute is assigned will be visualised. To turn-off the visualisation of the assignments, click the right-hand mouse button on the Thickness=15 material attribute name in the Treeview and select the Visualise Assignments option again from the dialog. Note. This method can be used at any time during this example to check that selected attributes have been correctly assigned to the model. Manipulating layers At any time the layers displayed in the redisplayed. • Treeview may be re-ordered, hidden or Treeview and Click the right-hand mouse button on the Mesh name in the select the Move Down option. The mesh can now be seen on top of the visualised geometry. At any time the mesh (and other features) displayed in the graphics window may be hidden or re-displayed. • With no features selected click the right-hand mouse button in a blank part of the graphics window and select the Mesh option. If a mesh was previously displayed it will be hidden, if previously hidden it will be displayed. This facility can be used to simplify the display when it is required. • Turn-off the display of the Mesh as described in the previous note. 27 Linear Elastic Analysis of a Spanner Fleshing Visualisation of assigned geometric attributes can also be seen using the fleshing option. Select the fleshing on/off button to turn-on geometric property visualisation. Select the isometric button to see the geometric visualisation on the elements. Select the dynamic rotate button to view the spanner from the side. The difference in thickness between the handle and the jaws can be seen. Select the fleshing on/off button to turn-off the geometric visualisation. Select the Home button to return the model to the default view. Reset to normal cursor mode. Supports LUSAS provides the more common types of support by default. These can be seen in the Treeview. Two support attributes are required, one which restrains movement in the X direction, and one which restrains movement in the Y direction. 28 Modelling : Attributes Assigning the Supports • Select the Point on the centreline of the spanner as shown to assign the support Fixed in X. Select these 2 Points for support 'Fixed in Y' • Drag and drop the support attribute Fixed in X from the Treeview onto the selected point. Select this Point for support 'Fixed in X' • Click the OK button to assign the support to the Point selected. The support will be visualised using an arrow symbol. Select the 2 Points shown to assign the support Fixed in Y. Hold the Shift key down to add the second point to the selection. • Drag and drop the support attribute Fixed in Y onto the selected points. • Click the OK button to assign the support to the points selected. The supports will be visualised using arrow symbols. • Click the left-hand mouse button in a blank part of the graphics window to deselect any previously selected model features. Defining the Loading A pressure load is to be distributed evenly along the top edge of the handle. Attributes Loading… > • Select the Face option and click Next 29 Linear Elastic Analysis of a Spanner • Enter loading of 0.1 in the y direction. • Enter the attribute name as Face Load of 0.1. • Click the Finish button to add the loading attribute to the Treeview. Assigning the Loading • Select the Line on the top edge of the spanner handle. Select this Line • Drag and drop the loading attribute Face Load of 0.1 from the Treeview onto the selected Line. • Click the OK button to assign the loading to the Line selected. Note. If the loading is displayed in the opposite direction to that shown the Surface forming the top half of the handle may be reversed as follows: • Select the Surface defining the top-half 30 Modelling : Attributes of the spanner by dragging a box around it. Geometry Surface Reverse... This will reverse the Surface axes and hence the direction of the loading. > Saving the model File Save To save the model file. Modelling Attributes Recap In this section, the attributes of the model were defined and assigned to the features. A regular Surface mesh with quadrilateral plane stress elements was defined and assigned to the jaws of the spanner. An irregular Surface mesh with triangular plane stress elements and a fixed element size was defined and assigned to the handle of the spanner. Two geometry attributes were used to specify the spanner jaws and handle thickness. A material attribute specifying the properties of steel was defined and assigned to all Surfaces. Two support attributes were defined in order to simulate the spanner being used to turn a nut and a structural face load was applied to the top edge of the handle. Attributes assigned to the model were checked visually for correct assignment. The model definition is now complete. The next step in the process is to run an analysis to solve the problem. 31 Linear Elastic Analysis of a Spanner Running the Analysis With the model loaded: File LUSAS Datafile... The data file name of spanner will be automatically entered in the File name field. With the Solve now option selected the LUSAS Solver will run an analysis. The Load results option ensures that the results from the analysis are loaded on top of the existing model for immediate use in results processing. • Click the Save button to create the LUSAS data file from the model information. Note. Pressing the Solve Now toolbar button also runs an analysis and automatically uses the values shown on the LUSAS Datafile dialog. If the analysis is successful... The LUSAS results file (spanner.mys) will be added to the Treeview. In addition, 2 files will be created in the directory where the model file resides: spanner.out this output file contains details of model data, assigned attributes and selected statistics of the analysis. spanner.mys this is the LUSAS results file which is loaded automatically into the Treeview to allow results processing to take place. If the analysis fails... If the analysis fails, information relating to the nature of the error encountered can be written to an output file in addition to the text output window. Any errors listed in the text output window should be corrected in LUSAS Modeller before saving the model and re-running the analysis. Note that a common mistake made when using 32 Viewing the Results LUSAS Modeller for the first time is to forget to assign particular attribute data (geometry, mesh, supports, loading etc.) to the model. Rebuilding a Model If it proves impossible for you to correct the errors reported a file is provided to enable you to re-create the model from scratch and run an analysis successfully. spanner_modelling.vbs carries out the modelling of the example. File New… Start a new model file. If an existing model is open Modeller will prompt for unsaved data to be saved before opening the new file. • Enter the file name as spanner File Script Run Script... File LUSAS Datafile... > To recreate the model, select the file spanner_modelling.vbs located in the \\Examples\Modeller directory. Rerun the analysis to generate the results. Viewing the Results In this section the results produced by the analysis of the spanner will be viewed. There are a number of ways to do this in LUSAS, allowing you to choose the most appropriate way to present your results. For this problem: A plot of the deformed mesh will be displayed and superimposed upon the undeformed shape for comparison. The principal stress vectors will be plotted. The von Mises stress contours for averaged stress values will be displayed. Peak values of von Mises stress will be marked. A graph will be produced showing the variation of stress along a slice section through the handle of the spanner. 33 Linear Elastic Analysis of a Spanner Selecting the results to be viewed If the analysis was run from within Modeller the results will be loaded on top of the current model and the first results loadcase (spanner.mys) is set active. This in the is signified by the results bitmap Treeview. Using Page Layout Mode The model was created using a Working Mode view which allows a model of any size to be created. Results could be viewed using this mode of operation, but in order to allow additional information to be added without obscuring the model, Page Layout Mode can be used instead. View Page Layout Mode... The graphics window will resize to show an A4 size piece of paper. File Page Setup... • Ensure that the Landscape option is selected and that left, right, top and bottom page Margins of 60, 10, 10, 10 respectively are set. • Click the OK button. This page layout view can also be saved for subsequent re-use with other models. Window Save View... • Enter the view name Landscape Page Layout. as • Click the OK button 34 Viewing the Results Deformed Mesh Plot To plot a deformed mesh the geometry and attribute layers will be deleted and the mesh and deformed mesh layers will be added to the Treeview. • With no features selected, click the right-hand mouse button in a blank part of the Graphics window and de-select the Geometry option to remove the geometry layer from the Treeview. • Repeat the operation to de-select the Attributes layer. • If the mesh layer is not present in the Treeview click the right-hand mouse button in a blank part of the Graphics window and select the Mesh option to add the mesh layer to the Treeview. Alternatively double click on the Mesh layer in the Treeview to display the mesh layer properties. The mesh layer is to be plotted in green. and a • Select dialog will appear showing the range of pens and colours in use. The mesh is currently drawn in a solid grey line style and is shown by the button with dashed outline. • Select the Green line pen. • Click OK to redraw the mesh in the new colour. • With no features selected, click the right-hand mouse button in a blank part of the Graphics window and select the Deformed mesh option to add the deformed mesh layer to the Treeview. The properties of the deformed mesh layer will be displayed. 35 Linear Elastic Analysis of a Spanner • Select the Mesh tab and Show ensure the quadratic effects button is selected. (This will draw the elements with curved rather than straight edges). • Click the OK button to display the deformed mesh on top of the undeformed mesh layer. Principal Stress Vector Plots Principal stresses can be plotted as vectors with different colours being used to signify tension and compression. The mesh layer is no longer required and it will now be removed. • With no features selected, click the right-hand mouse button in a blank part of the graphics window and de-select the Mesh option to remove the mesh layer from the Treeview. • Click the right-hand mouse button in a blank part of the graphics window and select the Vectors option to add the vectors layer to the Treeview. The vector properties dialog will be displayed. • Select Stress - Plane Stress vector results of Principal stresses from the entity drop down list. • Click the OK button to display the vector plot with tension vectors shown in red and compression vectors shown in blue. 36 Viewing the Results Creating New Windows As an alternative to adding and removing layers from the Treeview for each type of results to be displayed the multiple windows facility can be used. Window New Window A new window with default layers of Mesh, Geometry and Attributes will be created. The graphics window will resize to show an A4 size piece of paper. Window Load view On the Load View dialog choose to load the view into the Current Window and select the Landscape Page Layout view name from the drop down list and click OK • In the new window, click the right-hand mouse button in a blank part of the Graphics window and de-select the Geometry option to remove the geometry layer from the Treeview. • Repeat to remove the Attributes • If necessary, and using the same method, redisplay the Mesh layer. Click Close to accept the default properties. Setting a Results Loadcase for the New Window When creating a new window the default loadcase for the window is the Model data loadcase rather than the Results file loadcase. To ensure that results can be viewed in the new window the Results file loadcase must be set to be active again. Treeview click the right-hand mouse button on the Loadcase 1 results • In the file 1:spanner.mys and select the Set Active option. 37 Linear Elastic Analysis of a Spanner Von Mises Stress Contour Plot Contours of von Mises Stress (Equivalent Stress) may be plotted as lines or as colourfilled contour ranges. To display stress contours the contour layer needs to be added Treeview. to the • With no features selected, click the right-hand mouse button in a blank part of the active window and select the Contours option to add the contours layer to the Treeview. The contour plot properties dialog will be displayed. • Select Stress - Plane Stress contour results for the entity drop down list and equivalent stresses SE as the component. • On the same dialog select the Contour Display tab and ensure that the Contour key button is selected. • Click the OK button to display the contour plot of equivalent stress along with the contour key. Note. The order of the layers in the Treeview governs the order in which the layers are displayed. To see the mesh layer on top of the contours the mesh layer must be moved down Treeview list to a the 38 Viewing the Results position after the contour layer. • In the Treeview select the Mesh layer in Window 2, click the right-hand mouse button and select the Move Down option. (This can also be done by selecting the layer with the left-hand mouse button and dragging and dropping a layer name on top of another layer name). The mesh layer will then be displayed on top of the contour layer. Moving information on the annotation layer Annotation layer objects such as the contour key may be moved after their initial placement. • To select the contour key click on the key with the left-hand mouse button. • Now press and hold the left-hand mouse button down, drag the key to a suitable position on the screen, and release the mouse button to reposition it. Marking Peak Values • Deselect the contour key by clicking the left-hand mouse button in a blank part of the graphics window. • With no features selected click the right-hand mouse button in a blank part of the graphics window and select the Values option to add the values layer to the Treeview. The values properties dialog will be displayed. 39 Linear Elastic Analysis of a Spanner • Select Stress - Plane Stress contour results from the entity drop down list and Equivalent stresses SE as the component. • On the same dialog, select the Values Display tab and set Maxima values to display the top 1% of results. (This will show the peak stress value) • Click the OK button to display the contour plot with peak values marked. Use the Zoom in button to enlarge the view of the spanner to check the number obtained. Use the Home button to both resize the view and ensure the model lies in the XY plane in readiness for creating a slice section of results. Creating a Slice Section of Results Utilities Graph Through 2D... • Ensure the Snap to grid button is selected and a grid size of 10 is specified. • Click the OK button. 40 Viewing the Results • Click and drag the cursor as shown (at the X=40 location) to define a section slice through the handle of the spanner where it joins the jaws. Click here Drag to here This operation leads directly on to creating a graph using the graph wizard… Selecting the Slice Data Results to be Plotted In this example a graph is to be plotted of the variation in stress through the specified section of the spanner. The X axis results of distance through the spanner have been defined by the section slice. The Y axis results now need to be specified. • Select Stress - Plane Stress results from the entity drop down list and Equivalent Stress SE from the component drop down list. • Click the Next button to define the Y axis results. Title information for the graph is now to be added. 41 Linear Elastic Analysis of a Spanner • Enter the graph title as Stress at neck section • Enter the X axis label as Distance along section • Enter the Y axis label as Equivalent Stress (N/mm2) • Deselect the Show symbols button. • Click the Finish button to display the graph in a new window and show the values used in an adjacent table. Note. If the graph title or axes labels are left unspecified Modeller will use default names. To see the graph at the best resolution enlarge the window to a full size view. Note. The properties of the graph may be modified by clicking on the graph with the right-hand mouse button and selecting the Edit Graph Properties option. 42 Viewing the Results To exit from the Graph Through 2D option click the Select Any cursor button. The grid will be removed. This completes the example. 43 Linear Elastic Analysis of a Spanner 44 Description Calculating Section Properties of a Box Section For software product(s): With product option(s): All. None. Description The section properties of an arbitrary shaped box section are to be computed from the geometry of the section which is supplied as a DXF file. Units of N, mm, t, s, C are used. Objectives The required output from the analysis consists of: Section Properties of a box section Keywords Section Properties, Arbitrary Section, Holes, Local Library, Server Library Associated Files box_section.dxf DXF file containing geometry of section. 45 Calculating Section Properties of a Box Section Modelling Running LUSAS Modeller For details of how to run LUSAS Modeller see the heading Running LUSAS Modeller in the Examples Manual Introduction. Note. This example is written assuming a new LUSAS Modeller session has been started. If continuing from an existing Modeller session select the menu command File>New to start a new model file. Modeller will prompt for any unsaved data and display the New Model dialog. Creating a new model • Enter the file name as box_section • Use the Default working folder. • Enter the title as Box Section • Select units of N,mm,t,s,C from the drop down list provided. • Set the Startup template as None • Set the User Interface to Structural • Ensure the vertical axis is set to Z • Click the OK button. Discussion The arbitrary section property calculator within LUSAS Modeller computes the section properties of any open or closed section. Cross-sections are created either as a single regular or irregular surface, or as a group of surfaces. Any holes in a section must be defined as separate surfaces and any number of holes can be included. When calculating cross-sectional properties the extent of a hole must be defined using a surface because this will also be meshed by the section property calculator in order to generate the section properties for the complete section. Feature Geometry File Import... • Locate the box_section.dxf file in the \\Examples\Modeller directory and click the Import button to read in the DXF file and create the cross section geometry as shown below. 46 Modelling Merging Features Because the DXF data contains start and end points for each line two records are stored for each point when only one is required. The geometry must now be merged to remove the duplicate points from the model. To do this: • Select the whole model by typing Ctrl + A keys • Select the Merge defining geometry as well option and click the OK button. Geometry Merge Geometry... • Click the mouse button in a blank part of the Graphics Area to deselect the model geometry. Defining holes within a section This is done by first defining a surface that represents the total extent of the box-section, then defining a surface that represents the void or hole, and then selecting both the surrounding and inner surface to create the hole in the bounding surface. • Geometry Surface Lines… > Create a Surface from the selected Lines. • Geometry Surface Lines… > Drag a box around the whole model Box select the whole model Drag a box around the lines defining the void. Create a Surface from the selected Lines. Box select the lines defining the void 47 Calculating Section Properties of a Box Section Geometry Surface Holes Create > > • Select the outer Surface of the box-section and then the inner Surface representing the void. (Use the Shift key to pick the second Surface to add to the selection) • De-select Delete geometry defining holes. This ensures that the geometry defining the void remains as a Surface in its own right. This is important for section property calculation. Select these two surfaces A new singular Surface will be created, containing a void which itself is a Surface. This new surface containing the hole can be seen / checked by clicking in a blank part of the Graphics Window and then re-selecting the outer surface. Calculating Section Properties Utilities Section Property Calculator Arbitrary Section… > The units of the model as selected in the startup form N,mm,t,s,C will be displayed in the drop down list. Note. There is no need to compute the section properties in the units they are to be used in the analysis model because units conversion is carried out when the section properties are extracted from the section library if it is found to be required. • Click the Apply button, and after a short wait the calculated section properties will be displayed in the greyed boxes on the right-hand side of the form. • Click Cancel to close the dialog. 48 Modelling This completes the example. Note. The section properties may be added to the local or server section property libraries by selecting the appropriate option(s) prior to selecting the Apply button. Alternatively you can deselect the ‘Recompute section properties’ option after selecting the ‘Add local library’ or ‘Add server library’ options. By default the model name is entered as the Section Name. This can be modified if required. Notes on the automatic meshing used The mesh used to compute the properties of each of the surfaces is displayed in the graphics window. By default an element size is selected which will assign 15 elements to the longest side and a minimum of 2 elements is applied to the shorter sides. This mesh may be adjusted by deselecting the automatic mesh check box and changing the mesh size in the Treeview. Alternatively, the maximum element on the longest side may be adjusted by changing the ‘Max elts/line’ option as required prior to selecting the Apply button. As with all finite element models the more elements used the more accurate the results but the slower the calculation. A good compromise of 2 elements across all thin sections has been found to provide reasonable results without using excessive computation time. 49 Calculating Section Properties of a Box Section 50 Description Nonlinear Analysis of a Concrete Beam For software product: With product options: Any. Nonlinear. Description A nonlinear plane stress analysis is to be carried out on a model of a reinforced concrete beam. The reinforcement is provided in the lower face of the beam and has a total cross-sectional area of 400 mm2. The superposition of nodal degrees of freedom assumes that the concrete and reinforcement are perfectly bonded. It is assumed that the self-weight of the beam is negligible compared with the applied load and that the effects of any shear reinforcement can be ignored. All dimensions in millimetres 1200 BAR3 Elements C-L Point Load 450 QPM8 Elements 150 300 1650 1650 Due to the symmetrical nature of the problem, only the left-hand span of the beam is modelled. The beam is simply supported at the left-hand end with a symmetry support at the right-hand axis of symmetry. A concentrated vertical load is applied to the top of the beam 1200mm from the left-hand end. The concrete section is represented by plane stress (QPM8) elements, and the reinforcement bars are represented by bar (BAR3) elements. A nonlinear concrete cracking material model will be applied to the plane stress elements and a von Mises plastic material will be applied to the reinforcement bars. Units of N, mm, t, s, C are used throughout. 51 Nonlinear Analysis of a Concrete Beam Objectives The behaviour of the beam under cracking/yielding is to be examined by producing the following: A Deformed Mesh Plot showing the final deformed shape. A Load Displacement Graph for the top node on the axis of symmetry of the beam. Stress contour plot showing the stress distribution in the beam. Crack pattern plot showing the crack patterns produced. Animation of stresses and crack patterns for selected load increments. A graph of variation in stress through selected slice sections through the beam. Keywords 2D, Plane Stress, Bar Elements, Nonlinear Concrete Model, Element Selection, Concrete Cracking, Steel Reinforcement, Groups, Crack Patterns, Animation, Graphing, Load Displacement Curve, Slice Sections Associated Files beam_nl_modelling.vbs carries out the modelling of the example. Modelling Running LUSAS Modeller For details of how to run LUSAS Modeller see the heading Running LUSAS Modeller in the Examples Manual Introduction. Note. This example is written assuming a new LUSAS Modeller session has been started. If continuing from an existing Modeller session select the menu command File>New to start a new model file. Modeller will prompt for any unsaved data and display the New Model dialog. Creating a new model • Enter the file name as beam_nl • Use the Default working folder. 52 Modelling • Enter the title as Nonlinear Concrete Beam • Set the units as N, mm, t, s, C • Select the model startup template Standard • Select a Structural user interface. • Select the Vertical Y Axis option. • Click the OK button. Note. Save the model regularly as the example progresses. Use the Undo button to correct any mistakes made since the last save was done. Defining the Geometry Geometry Line Coordinates... > Enter coordinates of (0, 0), (1200, 0) and (1650, 0) to define two Lines representing the bottom of the left hand span of the beam. Click the OK button to finish. Drag a box to select these 2 Lines • Select both Lines just drawn by dragging a selection box around them. Geometry Surface By Sweeping... > Enter a translation value of 25 in the Y direction to create the Surface which represents the concrete cover from the face of the beam to the centreline of the reinforcement. • Click the OK button. • Select the upper Lines of both of the Surfaces just drawn as shown. Geometry Surface By Sweeping... > Select these 2 Lines Enter a translation value of 275 in the Y direction to create the Surface which represents the extent of the concrete above the centreline of the reinforcement. • Click the OK button. 53 Nonlinear Analysis of a Concrete Beam The model should appear as shown. Defining Groups To simplify the assignment of model attributes certain model features will be grouped together to allow selection by name in the Treeview as opposed to selection by cursor in the graphics window. The 2 Lines representing the reinforcement bars are to be grouped together: • Ensure the 2 Lines are still selected as shown. Geometry Group New Group Select these 2 Lines Enter Bars for the group name. > • Click the OK button to complete creation of the group. The Surfaces representing the concrete are to be grouped together. • Holding-down the S key, drag a box around the whole model to select only the Surfaces defining the concrete. Geometry Group New Group > Enter Concrete for the group name. Click the OK button to complete creation of the group. Drag a box to select only Surfaces Note. In this example, model attributes will be defined but not assigned to the model straight away. They will be assigned to the model later by making use of the Groups facility. Defining the Mesh - Reinforcement Bars Separate mesh datasets need to be defined for the reinforcement bars and the concrete. For the reinforcement bars a uniform mesh is to be used to the right of the applied load and a graded mesh is to be used on the horizontal lines to the left of the applied load. The reinforcement bars will be modelled using Line meshes. Attributes Mesh Line… > • Set Generic element type to Bar, Number of dimensions to 2 dimensional and Interpolation order to Quadratic 54 Modelling • Ensure the Number of divisions is set to 4 • Enter the attribute name as Bar Elements - Divs=4 • Click the Apply button to create the attribute in the dialog visible to allow additional datasets to be defined. Treeview and leave the • Change the Number of divisions to 6 and click the Spacing button. • Select a Uniform transition ratio of first to last element of 2 and click OK • Change the attribute name to Bar Elements - Divs=6 graded • Click the OK button to finish to add the attribute to the Treeview. Defining the Mesh - Concrete The concrete will be modelled using a Surface mesh with Line mesh divisions to control the mesh density. The default mesh density of 4 divisions per line is sufficient for the Surface to the right of the applied load. A graded line mesh will be created for use on the Surface to the left of the applied load. Attributes Mesh Surface… > • Select Plane stress, Quadrilateral, Quadratic elements. • Enter the attribute name as Plane Stress - Concrete • Click the OK button to add the attribute to the • In the Treeview. Treeview double click the Line mesh attribute name Divisions=6 The Line mesh properties dialog will appear. • Click the Spacing button. • Select Uniform transition ratio of first to last to first element of 2 and click OK • Change the attribute name to Divisions=6 graded • Click the OK button to add the attribute to the Treeview. Defining the Geometric Properties Attributes Geometric Line… > • Select Bar/Link from the drop down list and enter a value of 400 for the total cross sectional area of the reinforcement. • Enter the attribute name as Steel Area and click the OK button to add the attribute to the Treeview. 55 Nonlinear Analysis of a Concrete Beam Attributes Geometric Surface… > • Enter a value of 150 for the thickness. Leave the eccentricity blank. • Enter the attribute name as Beam Thickness and click the OK button to add the attribute to the Treeview. Defining the Material Properties Nonlinear steel properties will be defined for the reinforcing bar elements. Attributes Material Isotropic… > • Enter Young's modulus as 210e3 and Poisson's ratio as 0.3 and leave the mass density field blank. • Click the Plastic option and enter an Initial uniaxial yield stress of 300 • Select the Hardening option, click the Hardening gradient button and enter a hardening Slope value of 2121 with a Plastic strain of 1 • Enter the attribute name as Nonlinear Steel • Click the OK button to add the attribute to the Treeview. Nonlinear concrete material properties will be defined for the Surface elements representing the concrete. Attributes Material Isotropic… > • Enter a Young's modulus of 42000, a Poisson's ratio of 0.2 and leave the mass density field blank. • Click the Plastic option and from the drop-down list select the Concrete (model 94) entry. • Select the Reinforced concrete option • Enter a Uniaxial compressive strength value of 31.58 • Enter a Uniaxial tensile strength value of 3.158 • Change the Strain at end of softening curve to be 0.003 • Enter the attribute name as Nonlinear Concrete • Click the OK button to add the attribute to the Treeview. Assigning Attributes to the Bars The various Line and Surface mesh, geometric and material attributes defined previously will now be assigned to the model using the groups that have been defined. 56 Modelling • In the Treeview right-click the group name Bars. Select the Set as Only Visible option. The features in the group will be displayed. • Select the left hand Line of the two Lines representing the bars. Select this Line for Bar Elements - Divs=6 graded • Drag and drop the Line mesh attribute Bar Elements - Divs=6 graded from the Treeview onto the selected Line. Select this Line for Bar Elements - Divs=4 • Select the right hand Line of the two Lines representing the bars. • Drag and drop the Line mesh attribute Bar Elements - Divs=4 from the Treeview onto the selected Line. The Line mesh divisions will be defined with the spacing as shown. • Select both Lines. • Drag and drop the geometric attribute Steel Area from the Treeview onto the selected features. • Drag and drop the material attribute Nonlinear Steel from the the selected features. Treeview onto Note. The diagrams in this example show element nodes. To see these at any time you can go to the Treeview and double-click the Mesh layer. On the Mesh tab select Show nodes and click the Close button. Assigning Attributes to the Concrete • In the Treeview right-click the group name Concrete. Select the Set as Only Visible option. The Lines in the Bars group will be removed from the display and the Concrete group will be displayed. 57 Nonlinear Analysis of a Concrete Beam • Select the left-top and left-bottom Lines as shown. • From the Treeview drag and drop the Line mesh attribute Divisions=6 graded onto the selected features. Select this Line • Select the whole model using the Ctrl and A keys together. • Drag and drop the Surface mesh attribute Plane Stress - Concrete from the Treeview onto the selected features. ... and this Line A graded mesh will be drawn on the left-hand Surface and a uniform mesh will be drawn on the right-hand Surface. • Drag and drop the geometry attribute Beam Thickness from the Treeview onto the selected features. Select the fleshing on/off button to turn-off the geometric visualisation. If at any time during the example you wish to visualise the geometry select this button. • With the whole model still selected, drag and drop the material attribute Nonlinear Concrete from the Treeview onto the selected features. Ensure the Assign to surfaces option is selected and click OK The mesh on the Lines representing the cover to the centreline of the reinforcement needs to be altered. This is because they currently have a default Line mesh of 4 divisions per line when only 1 division per line is required. • Drag boxes to select the 3 Lines as shown. (Remember to hold the Shift key down after the first line is selected so the other lines are added to the selection) • Drag and drop the Line Drag 3 boxes to select these 3 Lines mesh attribute Divisions=1 from the Treeview onto the selected Lines. The mesh will be redisplayed with the revised mesh pattern. 58 Modelling Making all groups visible • From the Treeview right-click the group heading name beam_nl.mdl. Select the Set as Only Visible option. Click Yes to act on sub groups as well. All features in the model will now be displayed as shown. Supports LUSAS provides the more common types of support by default. These can be seen in the Treeview. The beam is to be simply supported in the Y direction at the lefthand end and a horizontal restraint in the X direction is required to satisfy the symmetry requirements at mid-span. • Select the lowest Point at the left hand end of the model as shown. Select these 2 Lines for support 'Fixed in X' • Drag and drop the support attribute Fixed in Y from the Select lower Point for Treeview onto support 'Fixed in Y' the selected Point. Ensure the Assign to points and All loadcases options are selected and click OK • Drag a box around the 2 Lines at the right hand end of the model as shown. • Drag and drop the support attribute Fixed in X from the Treeview onto the selected Lines. Ensure the Assign to lines and All loadcases options are selected and click OK Loading A single concentrated load is to be applied to the Point at the top of the beam. A unit load will be applied and the load factor in the nonlinear control will be used to control the magnitude of loading. Attributes Loading... • With the Concentrated option selected click Next • Enter a loading value of -1 in the component Concentrated load in Y Dir • Enter the attribute name as Point Load and click Finish 59 Nonlinear Analysis of a Concrete Beam • Select the Point on the top of the beam as shown. Select this Point • Drag and drop the loading dataset Point Load from the Treeview onto the selected Point. • Ensure the Assign to points option is set and click OK to assign the load to Loadcase 1 with a factor of 1 Nonlinear Control Nonlinear analysis control properties are defined as properties of a loadcase. The nonlinear analysis is to be terminated when the beam deflection at mid span reaches a limiting value. • Select the point shown. Select this Point • In the Treeview rightclick on Loadcase 1 and select Nonlinear & Transient from the Controls menu. 60 Modelling The Nonlinear & Transient dialog will appear: • Select the Nonlinear option and set Incrementation to Automatic • The initial load to be applied is the actual load applied to the model multiplied by the starting load factor. Set the Starting load factor to 5000 • Enter the Max change in load factor as 2000 to restrict the second and subsequent load increment sizes to ensure sufficient points are obtained to observe the load deflection behaviour of the beam. • Change the Max total load factor to 0 as the solution is to be terminated on the limiting displacement at mid span. • Change the number of desired Iterations per increment to 10 Note. If the number of iterations on the previous increment is less than the desired number the next load increment will be increased (up to the maximum change in load increment) while if the number of iterations is less than the desired number the next load increment will be reduced. • In the Solution strategy section of the dialog, ensure the Maximum number of iterations is set to 25 61 Nonlinear Analysis of a Concrete Beam • Leave the Residual force norm as 0.1 and the Incremental displacement norm to 1 so convergence of the solution at each load increment will be achieved when the out of balance forces are as less than 0.1% of the reactions and the iterative change in displacements is less than 1% of the displacements for that load increment. • Select the Advanced button in the Incrementation section of the dialog. • Ensure that the Stiffness ratio to switch to arc length value is set to 0.0 • Select the Terminate on value of limiting variable option. • The selected point number (this may differ depending on how the model was created) will appear in the Point number drop down list. • Set the Variable type to V to monitor the deflection at the selected point in the Y direction. • Enter a value of -3 so the analysis is terminated when the central deflection reaches this value. • In the Step reduction section ensure the Allow step reduction option is selected. • Click OK to return to the Nonlinear & Transient dialog. • Click OK again to set the loadcase properties. One additional setting is required for this analysis to ensure no element mechanisms are induced as the material yields. 62 Running the Analysis File Model Properties… • Select the Solution tab. • Click on the Element Options button and select the Fine integration for stiffness and mass option. • Click the OK button to return the Model Properties dialog. • Click the OK button to finish. Save the model The model is now complete and the model data is to be saved before an analysis is run using the LUSAS Solver. File Save Save the model file. Running the Analysis With the model loaded: File LUSAS Datafile... A LUSAS data file name of beam_nl will be automatically entered in the File name field. • Ensure that the options Solve now and Load results are selected. • Click the Save button to finish. During the analysis 2 files will be created: beam_nl.out this contains the statistics of the analysis, for example how much disk space was used, how much CPU time was used, and any errors or warning messages from LUSAS, and so on. Always check the LUSAS output file for error messages. beam_nl.mys this is the LUSAS results database which will be used for results processing. If the analysis is successful... The LUSAS results file will be displayed in the 63 Treeview. Nonlinear Analysis of a Concrete Beam If the analysis fails... If the analysis fails, information relating to the nature of the error encountered can be written to an output file in addition to the text output window. Select No to not view the output file. Any errors listed in the text output window should be corrected in LUSAS Modeller before saving the model and re-running the analysis. Rebuilding a Model If it proves impossible for you to correct the errors reported a file is provided to enable you to re-create the model from scratch and run an analysis successfully. beam_nl_modelling.vbs carries out the modelling of the example. File New… Start a new model file. If an existing model is open Modeller will prompt for unsaved data to be saved before opening the new file. • Enter the file name as beam_nl File Script Run Script... File LUSAS Datafile... > To recreate the model, select the file beam_nl_modelling.vbs located in the \\Examples\Modeller directory. Rerun the analysis to generate the results. Viewing the Results If the analysis was run from within LUSAS Modeller the results will be loaded on top of the current model and the loadcase results for load increment 1 are set to be active by default. Changing the Active Results Loadcase • In the Treeview right-click on the last load increment Increment 9 Load Factor = 16972.6 and select the Set Active option. Deformed Shape • If present in the Treeview delete the Geometry, Attributes and Mesh layers to clear the display. 64 Viewing the Results • With no features selected, click the right-hand mouse button in a blank part of the graphics window and select the Deformed mesh option to add the deformed mesh layer to the Treeview. • Click OK to accept the default properties and view the deformed mesh for the final load increment. Creating a Load versus Displacement Graph A graph of displacement at mid-span is to be plotted against the applied load. To do this a node on the line of symmetry is selected: Select this Node • With the Deformed mesh layer visible, select the top node on the axis of symmetry as shown. Using the Graph Wizard The graph wizard provides a step-by-step means of selecting which results are to be plotted on the X and Y axes of the graph. The X axis is always defined first. Utilities Graph Wizard... • Ensure the Time history option is selected and click the Next button. • Ensure the Nodal results is selected and click Next • Select entity Displacement for component resultant displacement RSLT • The node number selected earlier will be displayed in the drop-down list. • Click the Next button. The Y axis results to be graphed are now defined. • Select the Named option and click Next • Select Total Load Factor from the drop down list. 65 Nonlinear Analysis of a Concrete Beam • Click the Next button. • Leave all title information blank and click the Finish button to display the load deformation graph. Note. Graphs can be modified using the right hand mouse button in the graph window and selecting the Edit Graph Properties option. Close the graph window. Use the maximise button to increase the size of the graphics window. Maximum Principal Stress Contour Plots • Delete the Deformed mesh layer from the Treeview. • With no features selected, click the right-hand mouse button in a blank part of the graphics window and select the Contours option to add the contours layer to the Treeview. The properties dialog will be displayed. • Select entity Stress Plane Stress for component of stress in the x direction, SX • Click the OK button to display contours of stresses for the final load increment. Viewing Crack Patterns • With no features selected, click the right-hand mouse button in a blank part of the graphics window and select the Vectors option to add the vectors layer to the Treeview. The properties dialog will be displayed. • Select Stress - Plane Stress contour results of type Crack 66 Viewing the Results • Select Vector Display tab and for the Tension vectors select the Choose Pen option and change the line colour to Black • Select the Scale tab and with the Use local scale option selected specify a magnitude of 2 • Click the OK button to display the cracking pattern for final load increment superimposed onto the stress contours. Animating the Results As an alternative to viewing results individually for each loadcase, the change of stress due to the increasing load increments can be animated instead. To ensure consistent contour values throughout the animation the interval of the range of contours is to be specified. • In the Treeview double-click on the Contours layer. The contour properties will be displayed. • Select the Contour Display tab and deselect the Contour key option to remove the key from the display. • Select the Contour Range tab and click the Interval option and set the contour interval as 1 • Click the Maximum button and set the maximum value as 3 • Click the Minimum button and set the minimum value as -16 • Click the Set as global range and Use global range options. • Click the OK button to redisplay the stress contours using the new contour range. Using the Animation Wizard Utilities Animation Wizard... • Select the Load History option and click the Next button. • Select beam_nl.mys from the drop-down list. 67 Nonlinear Analysis of a Concrete Beam • Select the All loadcases option and select the Finish button to create the animation sequence. Note. The buttons at the bottom of the window may be used to slow-down, speed-up, pause, step through frame by frame, or stop the animation. Saving Animations Animations may be saved for replay in Windows animation players. • Ensure the animation window is the active window. File Save As AVI... • Browse to your projects folder and enter beam_nl for the animation file name. An .avi file extension is automatically appended to the file name. Click Save • Animations can be compressed to save disk space. A number of compression formats are available depending on what is installed on the system. Microsoft Video 1 has been found to provide reliable results. Click OK Close the animation window, choosing not to save changes. Enlarge the model window to a full size view. 68 Viewing the Results Creating a slice section of results In this example a graph is to be plotted of the variation in stress through the specified section of the beam. The X axis values of distance are defined by the section slice. The Y axis results are specified from the graph wizard dialog. Utilities Graph Through 2D • Ensure the Snap to grid option is selected and a grid size of 100 is specified. • Click the OK button. Note. The snap to grid dialog will only appear if the model is viewed in the XY plane. If necessary, return the model to the default starting view by clicking on the status bar at the bottom of the graphics window. • Using the screen ruler as a guide, click and drag the cursor as shown to define the location of a section slice through the beam at a distance of 1600 from the left-hand end. • Select Stress - Plane Stress results for Stress SX and click the Next button. • Leave all title information blank. • Click the Finish button to create the graph of stress through the section of beam. 69 Nonlinear Analysis of a Concrete Beam Adding Additional Results to a Graph Window 1 LUSAS View beam_nl.mdl Window 1 • Re-select the window containing the results contours. The cursor will still be in section slice mode. • Using the screen rulers as a guide, click and drag the cursor as shown to define the location of a section slice through the beam at a distance of 1000 from the left-hand end. • Select Stress - Plane Stress results for Stress SX and click the Next button. • Click the Add to existing graph option. • Click the Finish button to add the results for the second slice section to the existing graph. This completes the example. 70 Description : Linear Material Contact Analysis of a Lug For software product(s): With product option(s): All. Nonlinear (for the second part of the example) Description : Linear Material A large lug is supported at its left-hand edge and subjected to a prescribed pressure load around the inside of the hole, modelling a loaded pin. 1.5 1.0 0.75 R = 0.5 Loading 0.75 The lug is 0.546 m thick and made of steel with a Young's modulus of 210E9 N/m2, a Poisson's ratio of 0.3 and a mass density of 7800kg/m3. A linear static analysis is carried out initially. Material properties and loading are then modified to investigate the response of the lug using a nonlinear analysis. Units used are N, m, kg, s, C throughout. Objectives The output required from the analysis consists of: Deformation Plot A plot of the undeformed and deformed mesh. Contour Plot A Von Mises stress plot. 71 Contact Analysis of a Lug Principal Stress Vectors A plot of principal stress vectors. Fatigue Damage A plot of the fatigue damage when the component is subjected to a prescribed loading sequence. Cycles to Failure A contour plot of the number of cycles to failure for the area around the hole. Keywords 2D, Default Assignments, Linear, Slideline, Nonlinear, Contact, Fatigue, Damage, Cycles to Failure, Stress Contours, Displacement Results, Animation, Graph Plotting. Associated Files lug_linear_modelling.vbs carries out the modelling for the linear analysis. lug_nonlinear_modelling.vbs carries out the modelling for the nonlinear contact analysis. Modelling : Linear Material Running LUSAS Modeller For details of how to run LUSAS Modeller see the heading Running LUSAS Modeller in the Examples Manual Introduction. Note. This example is written assuming a new LUSAS Modeller session has been started. If continuing from an existing Modeller session select the menu command File>New to start a new model file. Modeller will prompt for any unsaved data and display the New Model dialog. Creating a new model • Enter the file name as lug_linear • Use the Default working folder. • Enter the title as Fixing Lug (Linear analysis) • Set the units to N,m,kg,s,C • Select the startup template Standard • Select a Structural user interface. 72 Modelling : Linear Material • Specify the vertical axis in the Y direction. • Click the OK button. Note. Save the model regularly as the example progresses. Use the Undo button to correct any mistakes made since the last save was done. Default Attribute Assignments The material properties of the lug, its element type and thickness are uniform over the model. Default attribute assignments can therefore be used, meaning that any material, mesh or geometry attribute defined will be automatically assigned to any features that are subsequently generated. Default Element Selection The lug is a relatively thin structure and all deformations take place in the plane of the structure therefore plane stress continuum elements will be used. Attributes Mesh Surface… > • Select Plane stress, Quadrilateral, Quadratic elements. Ensure the Regular mesh option is selected with Automatic mesh divisions so that LUSAS uses the default number of mesh divisions on each line. Leaving the attribute name blank causes LUSAS to create a suitable default attribute name. Click OK Modeller will add the Surface Mesh 1 attribute to the Treeview. • To make this attribute the default for all subsequent geometry, click the right-hand mouse button on the mesh attribute Surface Mesh 1 in the Treeview and select the Set Default option. The selected attribute will be highlighted to signify that it has been set as the default for all subsequent features. Default Geometric Properties Attributes Geometric Surface... > • Enter the thickness as 0.546. No eccentricity needs be entered. • Enter the attribute name as Lug Thickness 0.546 and click OK. • To make this attribute the default for all subsequent geometry click the right-hand mouse button on the geometry attribute name in the Treeview and select the Set Default option. 73 Contact Analysis of a Lug Default Material Properties Attributes Material > Material Library… • Select material Mild Steel from the drop down list, leave the units as N,m,kg,s,C and click OK to add the material attribute to the Treeview. • To make the mild steel material attribute the default for all subsequent geometry click the right-hand mouse button on the Mild Steel Ungraded (N,m,kg,s,C) material attribute name in the Treeview and select the Set Default option. Defining the Geometry Use will be made of the symmetry of the lug by defining the top half and then mirroring it to form the whole structure. In this problem the centre of the hole will be taken as the origin (0,0,0). Geometry Surface Coordinates… > Define a Surface by specifying the coordinates of its vertices using the following values (-2.5, 0), (-1, 0), (-1, 0.75) and (-2.5, 0.75). Select the fleshing on/off button to turn-off geometric property visualisation. Note. Whenever a Surface is created the corresponding Surface mesh will be displayed. For clarity the diagrams accompanying this example will not generally show the mesh. At any time the mesh can be removed or added to the display as follows: With no features selected click the right-hand mouse button in a blank part of the Graphics window and select the Mesh option. If a mesh was previously displayed it will be hidden. If previously hidden it will be displayed. Geometry Line Coordinates… > Define a Line by specifying the coordinates of either end as (0.5, 0) and (0.75, 0). The resulting features should be as shown. Note. LUSAS will automatically generate any necessary lower order features when higher order features are defined. New Surfaces will be created by sweeping the Line just drawn through a positive (anti-clockwise) angle about the centre of the hole. • Select the new Line. 74 Modelling : Linear Material Geometry Surface > By Sweeping… Rotate the Line through an angle of 45 degrees about the Zaxis and an origin of (0,0,0) to sweep through a Minor arc to create the surface. Copy this Surface to form next Surface Select this Line to form first Surface • Enter the attribute name as Rotate 45 Degrees so that it can be re-used. • Click on the Save button to save the attribute information and click the OK button to finish. LUSAS will create a new Surface from the selected Line. This will now be copied to create the adjoining surface. • Select the Surface just created. Geometry Surface Copy… > On the Copy dialog, select the Rotate 45 degrees attribute from the drop-down list to use the values defined. • Click the OK button to create the new Surface. 3. Drag a box to select these 2 Points The arc forming the Surface of the hole is to be extended. • First, select Point shown. Geometry Line > Arc/Circle > By Sweeping Points… the 2. Select this Point to create second arc. 1. Select this Point to create first arc. Select the Rotate 45 degrees attribute from the drop-down list to use the values defined. • Click the OK button to create the new arc. • Secondly, select the Point at the end of the new arc and repeat the previous process to draw a second arc. • Thirdly, drag a box around the two unconnected Points at the top of the model. 75 Contact Analysis of a Lug Select the new Line button to create the connecting Line. Two new Surfaces will now be formed by joining existing Lines. • Select the first two Lines required in the order shown remembering to use the Shift key to add to the initial selection. Geometry Surface By Joining... > • Use the joining function, to create a surface between the specified lines. 1. Select this Line 2. Select this Line 3. Select menu option 4. Select this Line 5. Select this Line 6. Select menu option • Repeat for the remaining two Lines as shown. The top half of the lug is now complete. Mirroring the Lug The bottom half of the lug is to be formed by mirroring the top half. • Select 2 Points on the centreline. Edit Selection Memory > Set The points are stored in memory. Select these 2 Points to define mirror plane • Drag a box around the whole of the top half of the lug or use the Ctrl + A keys together to select the whole model. Geometry Surface Copy... > Edit Selection Memory > Clear Select the Mirror – from Point 1 and Point 2 from the drop down list and click the Use button to use the mirror transformation defined. Click the OK button to finish. The surfaces will be copied and mirrored. The points are cleared from selection memory. Note. As a consequence of mirroring the Surfaces, the orientation of the Surfaces in the top half of the model will be opposite to the orientation of the Surfaces in the bottom half of the model. The orientation of the Surfaces must therefore be checked. 76 Modelling : Linear Material Aligning Surface axes To ensure the loading directions are consistent the element axes should be aligned. The element axes follow the direction of the surface they are generated from. These may vary depending upon how your surfaces were created. Treeview right click on • In the Geometry and select Properties • On the properties dialog select the Surface axes button and click OK to display the surface axes. The axes of all surfaces can be aligned to axes of the first surface in the selection using the cycle relative facility. • Select the top left-hand surface. • Hold the Shift key and box-select the whole model to add the remaining surfaces to the selection. Geometry Surface Cycle Relative > The axes of all surfaces will be aligned to the axes of the first element selected. Treeview right click on • In the Geometry and select Properties • On the properties dialog deselect the Surface axes button and click OK to remove the surface axes from the display. Supports LUSAS provides the more common types of support by default. These can be seen in the Treeview. 77 Contact Analysis of a Lug • Drag a box around the 2 vertical Lines on the left of the model. • Drag the support attribute Fixed in XY from the Treeview and drop onto the selected Lines in the graphics window. Drag a box to select these 2 Lines • Choose options to Assign to lines for All loadcases and click OK to finish assigning the support attribute. The supports will be visualised as arrows at the supported nodes in the directions of the restraints. Loading In this linear analysis, pin loading is to be approximated by defining a face load of a value equivalent to the full load that will be applied during the nonlinear analysis. The face load will be assigned to the 2 Lines defining the lower side of the hole. Note. Face loads are applied in local element directions, hence a load in the Y direction will act in a radial direction. Attributes Loading… • Select the Face option and click Next • Input a load value of 10e6 in the Component y direction. • Enter the attribute name as Face Load and click Finish to add the attribute to the Treeview. • Select the 2 arcs forming the lower side of the hole, then drag and drop the Face Load attribute from the Treeview onto the selected features. • Ensure that Loadcase 1 and a Load factor of 1 are used and that the loading is assigned to Lines only. Select these 2 Lines • If not already displayed, turn on the display of the mesh. 78 Running the Analysis : Linear Material Saving the model File Save Save the model file. Running the Analysis : Linear Material With the model loaded: File LUSAS Datafile... A LUSAS data file name of lug_linear will be automatically entered in the File name field. • Ensure that the options Solve now and Load results are selected. • Click the Save button to finish. A LUSAS Datafile will be created from the model information. The LUSAS Solver uses this datafile to perform the analysis. If the analysis is successful... The LUSAS results file will be added to Treeview. In addition, 2 files will be created in the directory where the model file resides: lug_linear.out this output file contains details of model data, assigned attributes and selected statistics of the analysis. lug_linear.mys this is the LUSAS results file which is loaded automatically into the Treeview to allow results processing to take place. If the analysis fails... If the analysis fails, information relating to the nature of the error encountered can be written to an output file in addition to the text output window. Any errors listed in the text output window should be corrected in LUSAS Modeller before saving the model and re-running the analysis. Rebuilding a Model If it proves impossible for you to correct the errors reported a file is provided to enable you to re-create the model from scratch and run an analysis successfully. lug_linear_modelling.vbs carries out the modelling of the example. 79 Contact Analysis of a Lug File New… Start a new model file. If an existing model is open Modeller will prompt for unsaved data to be saved before opening the new file. • Enter the file name as lug_linear File Script Run Script... File LUSAS Datafile... > To recreate the model, select the file lug_linear_modelling.vbs located in the \\Examples\Modeller directory. Rerun the analysis to generate the results. Viewing the Results : Linear Material If the analysis was run from within LUSAS Modeller the results will be loaded on top of the current model and the loadcase results for Loadcase 1 are set to be active by default. For clarity, the lug geometry will be removed from the display to leave only the undeformed mesh displayed. • If present, delete the Geometry and Attributes layers from the Treeview. Using Page Layout Mode The model was created using a Working Mode view which allows a model of any size to be created. Results could be viewed using this mode of operation, but, in order to allow additional information to be added without obscuring the model, Page Layout Mode can be used instead. View Page Layout Mode The Graphics window will resize to show the mesh layer on an A4 size piece of paper. File Page Setup... • Ensure that the Landscape option is selected, ensure that page margins of 60,10,10,10 are set for left, right, top and bottom margins respectively and click OK This page layout view can also be saved for subsequent re-use with other models. Window Save View... • Enter the view name as Landscape Page Layout and click OK 80 Viewing the Results : Linear Material Deformed Mesh Plot • Delete the Mesh layer from the Treeview. • With no features selected click the right-hand mouse button in a blank part of the Graphics window and select the Deformed mesh option to add the deformed mesh layer to the Treeview. • Click on the OK button to accept the default properties and display the deformed mesh. Von Mises Stress Contours • With no features selected click the right-hand mouse button in a blank part of the graphics window and select the Contours option to add the contours layer to the Treeview. The contour layer properties will be displayed. • Select Stress - Plane Stress contour results of equivalent stresses SE • Click the OK button to display the contours and annotated contour summary. Note. The order of the layer names in the Treeview determines the order in which the layers will be displayed in the graphics window. To ensure a particular layer is displayed after another layer, click on the layer name to be moved in the Treeview and drag the layer name onto the layer name after which it is to be displayed. The display in the graphics window will be updated accordingly. • Move the Deformed mesh layer to follow the Contours layer in the Treeview as described in the previous note. 81 Contact Analysis of a Lug Marking Peak Values • With no features selected click the right-hand mouse button in a blank part of the Graphics window and select the Values option to add the values layer to the Treeview. The values properties will be displayed. • Select Stress - Plane Stress contour results of Equivalent stresses SE • Select the Values Display tab and set Maxima values to display the top 1% of results on the Deformed shape. • Click the OK button to redisplay the contours with the peak value marked. Principal Stress Vectors • Delete the Contours and Values layers from the Treeview. • With no features selected, click the right-hand mouse button in a blank part of the Graphics window and select the Vectors option to add the vectors layer to the Treeview. The vector layer properties will be displayed. • Select Stress - Plane Stress vector results. • Click the OK button to display vectors with tension vectors displayed in red and compression vectors displayed in blue. Defining a Fatigue Spectrum • Delete the Vectors layer from the Treeview. Utilities Fatigue… 82 Viewing the Results : Linear Material • Ensure lug_linear.mys is selected from the drop-down list. • Select Loadcase 1 • Click the ‘Add to’ button to include Loadcase 1 in the fatigue load spectra calculation. • Click on Loadcase 1 in the Included panel of the dialog and enter the number of Cycles as 10000 • Leave the name as Fatigue 1 and select Sabs from the component drop-down list. • Select the S N Curve tab and enter the values as shown in the table. • Click the OK button to finish. Log Stress/ Strain • In the Treeview right-click on the loadcase Fatigue 1 and select the Set Active option. Log Cycle 4.7323 15 9.7323 0 Contouring Damage Contouring damage must be done on an undeformed mesh view. • Delete the Deformed mesh layer from the Treeview. • With no features selected click the right-hand mouse button in a blank part of the graphics window and select the Mesh option to add mesh layer to the Treeview. Click OK to accept the default properties. • With no features selected click the right-hand mouse button in a blank part of the graphics window and select the Contours option to add the contours layer to the Treeview. 83 Contact Analysis of a Lug The contour plot properties will be displayed. • Select Stress - Plane Stress and ensure contour results of Damage are selected. • Select the Contour Display tab and ensure the Contour key option is selected. • Click the OK button to display contours of damage and a contour summary. • Move the Mesh layer to follow the Contours layer in the mesh is visible on top of the contour display. Treeview so the Contouring Cycles to Failure Modeller can calculate the number of repeats of a given loading sequence to failure. An extra fatigue spectrum will be created containing only a single loading cycle. Utilities Fatigue… • Ensure lug_linear.mys is selected from the drop-down list. • Select Loadcase 1 • Click the calculation. ‘Add to’ button to include Loadcase 1 in the fatigue load spectra • Leave the name as Fatigue 2 and select Sabs from the component drop-down list. • Select the S N Curve tab and enter the values as shown in the table. • Click the OK button to finish. In the Treeview right-click on the loadcase Fatigue 2 and select the Set Active option. • In the Log Stress/ Strain Log Cycle 4.7323 15 9.7323 0 Treeview double-click on the Contours layer. The contour plot properties will be displayed. • Select Stress - Plane Stress contour results of Damage • Click the Close button to display the contours and a summary of cycles to failure. • Double-click on the Contours layer again. 84 Viewing the Results : Linear Material • Select entity Stress - Plane Stress contour results of component Log-Life • Click the OK button to display contours of log life. Changing the levels The contours of log-life will be easier to understand if the contour levels are adjusted so that they are plotted in unit (1.0) increments, representing 10 to the power of 0 cycles to failure. Treeview, double-click • In the on the Contours layer name and select the Contour Range tab. • Set the Contour range to show a contour Interval of 1. Ensure the Value to pass through is set to 0 • Click the OK button to display contours of Log Life and a contour summary using the increments specified. A maximum value of 14.78 should be obtained for the log-life. This completes the linear analysis section of the example. 85 Contact Analysis of a Lug Description : Nonlinear Material This part of the example extends the previously defined lug model used for the linear analysis. The pressure loading is removed and an additional pin of 0.9m diameter is defined. Slidelines are defined on the surfaces that will come into contact and the pin is then subjected to a prescribed concentrated loading and moved into contact with the lug. A schematic of the lug and pin geometry is shown. The units of the analysis are N, m, kg, s, C throughout. Objectives The output required from the analysis is as follows: Equivalent Stress Contours A plot of the stress in the lug only. Graph of Displacement against Applied Load A graph of the resultant displacement at a selected node. Modelling : Nonlinear Material If the linear analysis was successful: File Open... File Save As... Open the model file lug_linear.mdl saved after completing the first part of this example • Enter the model file name as lug_nonlinear and click the Save button. • In the Treeview, right-click on results file lug_linear.mys and select Close file Note. Closing all results files also unlocks the mesh allowing re-meshing to take place. 86 Modelling : Nonlinear Material Rebuilding model from a supplied file If the linear analysis was not successful a file is provided to enable you to re-create the model for use in this part of the example. File New… Start a new model file. If an existing model is open Modeller will prompt for unsaved data to be saved before opening the new file. • Enter the file name as lug_nonlinear File Script Run Script... > To recreate the model, select the file lug_linear_modelling.vbs located in the \\Examples\Modeller directory. Changing the model description File Model Properties… • Change the model title to Fixing Lug - Nonlinear Contact Analysis and click OK • If present, delete the Contours and Annotation layers from the Treeview. • Ensure the Geometry layer is present. • In the Treeview set Loadcase 1 to be active. Feature Geometry For clarity the diagrams accompanying this example will not generally show the mesh. • Drag a box around the whole of the model (or use the Ctrl + A keys) to select the whole model. Select the group button to create a group. • Enter the name Lug and click OK to finish creating the group and add it to the Treeview. 87 Contact Analysis of a Lug • Select the Line on the lug shown. Take care to not include any other features. Geometry Line Copy... > Select this Line Select the Scale option and enter a scale factor of 0.9 • Click the OK button to create the arc. Geometry Point Coordinates... > Enter coordinates of (0, 0) to define a point at the origin and click OK • Select the Line just created and holding the Shift key down, also select the point at the origin. Geometry Surface By joining... > A new Surface will be created. The other surfaces of the pin will be created shortly. 1. Select this Line 2. Press Shift key 3. Select this Point Modifying the Line mesh divisions The total number of mesh divisions on the Pin is to be reduced and modified. • Ensure the mesh layer is displayed. • Select the arc on the initial segment of the pin. • Drag and drop the Line mesh attribute Divisions=2 from the Treeview onto the selected Line. Attributes Mesh Line… > • With the Element description set as None, enter the number of divisions as 2 • Click the Spacing button, select a Uniform transition ratio of last to first element of 0.333 and click OK to return to the mesh dialog. • Enter the attribute name as Divisions=2(3:1) and click OK LUSAS will add the attribute name to the Treeview. 88 Assign 'Divisions=2' to this Line Assign Line mesh 'Divisions=2(3:1)' to these 2 Lines Modelling : Nonlinear Material • Select the 2 straight Lines on the first surface of the Pin. • Drag and drop the Line mesh attribute Divisions=2(3:1) from the onto the selected features. Treeview Note. The last/first element spacing ratio depends upon the direction of the Line on which it is assigned. If the mesh is finer at the centre of the Pin than at the edge then reverse the line(s) by first selecting with the mouse and using the menu command Geometry>Line>Reverse The remainder of the Pin is to be generated by copying the initial segment of the Pin. • Select the Surface defining one-eighth of the Pin. Geometry Surface Copy… > From the drop-down list, select the attribute Rotate by 45 degrees • Set the number of copies to 7 • Click the OK button to create the new Surfaces forming the entire pin. Using Groups To allow easy selection of the features defining the pin, the group named Lug is to be hidden. • In the Treeview right-click on the group name Lug and select the Invisible option to leave just the Surfaces representing the pin displayed. • Drag a box around the features defining the pin (or use the Ctrl + A keys). Select the group button to create a group. • Enter the name Pin and click OK to finish creating the group and add it to the Treeview. Geometric properties of the pin Attributes Geometric Surface... > • Enter the thickness as 10 and the attribute name as Pin Thickness 10. Click OK • Box-select the Pin in the Graphics Area and drag and drop this geometric dataset from the Treeview onto the selected features 89 Contact Analysis of a Lug Redisplay the lug • In the Treeview right-click on the group name Lug and select the Visible option to re-display the lug. Modifying the mesh Contact problems using slidelines require linear rather than quadratic elements to be used. • In the Treeview double-click on the Surface Mesh 1 attribute name. • Change the interpolation order to Linear and click OK to overwrite the previous mesh details. • If not already displayed, display the mesh layer. The mesh arrangement should be as shown. Slidelines Slidelines define the contacting Surfaces of the model. They are used in pairs (a master and a slave) and define opposing contacting Surfaces. They are assigned to Lines for 2D analyses and to Surfaces for 3D analyses. In this analysis, the master and slave slides are assigned to selected internal Lines of the Lug and selected external Lines of the Pin. Attributes Slideline... • Ensure that the Close Contact parameter is set to 0.1 and leave the remaining values as their default settings. • Enter the attribute name as Lug_Pin and click OK 90 Modelling : Nonlinear Material • Select the 4 internal lower arcs of the Lug. • Drag and drop the slideline attribute Lug_Pin from the Treeview onto the selected features, setting this slideline to be the Master. Leave the orientation as Default and click OK Select these 4 Lines for Slave slideline Select these 4 Lines for Master slideline • Select the 4 lower arcs of the Pin. Treeview onto the • Drag and drop the slideline attribute Lug_Pin from the selected features, setting this slideline to be the Slave and click OK • To visualise the slidelines assigned to the model click the right-hand mouse button on the slideline attribute name in the Treeview and select Visualise Master Assignments and Visualise Slave Assignments • After visualising, de-select the visualisation of both sets of slidelines. Supports and Loads The loading from the first part of this example is to be removed and will be replaced by a concentrated load. The supports will remain unaltered. Treeview click the right-hand mouse button on the loading attribute • In the Face load. Select the Deassign > From all option. Attributes Loading... • With the Concentrated option selected click Next • Input a load in the Y direction of -2e8. • Enter the load attribute name as Concentrated Load and click the Finish button. 91 Contact Analysis of a Lug • Select the Point at the centre of the Pin. • Drag and drop the loading attribute Concentrated Load from the onto the selected point, ensuring that it is applied as Loadcase 1 Treeview Preventing features from merging together Now that the modelling is complete the pin can be moved into contact with the lug. This could be done by entering a known dimension, or, as shown in this example, by selecting the Points to be brought into contact. To prevent the features in the pin merging with those on the lug when the pin is moved into contact the points in the pin are set as unmergable. • Select all the features in the pin by selecting Pin in the the Select Members option. Geometry Point > Make Unmergable Treeview and picking This ensures the points in the pin are not merged with those in the lug. Moving the Pin to touch the Lug • Select the lowest Point on the Pin. Make a note of the Point number selected in the text output pane. 1. Select this Point • Holding the Shift key down, select the Point 2. Select this Point immediately beneath it on the hole of the Lug. Make a note of the Point number shown in the Selected box of the status bar. • Click the right-hand mouse button and select the Selection Memory>Set option. Treeview right-click on the group name Pin and select the Select • In the members option to highlight all features representing the pin. Click OK to deslect the previously selected Points. Geometry Point Move… > Select the Translation – from Point 45 to point 30 transformation (or the one that relates to your selected points) from the drop down menu and click the Use button to use the distance between the Points stored in memory as the move distance. Click the OK button to finish. The pin will be moved to rest against the lug at the starting point of the analysis. 92 Modelling : Nonlinear Material Nonlinear Analysis Control Nonlinear analysis control properties are defined as properties of a load case. Treeview right-click on Loadcase 1 and select the Nonlinear and • In the Transient option from the Controls menu. The Nonlinear & Transient dialog will appear: • Select Nonlinear incrementation with Automatic control. • Enter the Starting load factor as 0.001 • Enter the Max change in load factor as 0.5 • Enter the Max total load factor as 2 • Ensure that Adjust load based on convergence is selected. • Enter the number of Iterations per increment as 6 • Enter the Maximum time steps or increments as 100 • Click the OK button to finish. Note. A nonlinear contact analysis performs best when a small amount of load (0.001 of the load in this example) is applied to the model initially. Thereafter, once 93 Contact Analysis of a Lug the results for a load increment have been obtained the load factor for the next increment is automatically adjusted by LUSAS based upon the number of iterations taken for the previous load increment to converge. After a number of such iterations the loading will be progressively applied to the model until the total load factor is reached. Saving the model The model is now complete and the model data is to be saved before an analysis is run using the LUSAS Solver. File Save To save the model. Running the Analysis : Nonlinear Material With the model loaded: File LUSAS Datafile... A LUSAS data file name of lug_nonlinear will be automatically entered in the File name field. • Ensure that the options Solve now and Load results are selected. • Click the Save button to finish. During the analysis 2 files will be created: lug_nonlinear.out this contains the statistics of the analysis, for example how much disk space was used, how much CPU time was used, and any errors or warning messages from LUSAS, and so on. Always check the LUSAS output file for error messages. lug_nonlinear.mys this is the LUSAS results database which will be used for results processing. If the analysis is successful... The LUSAS results file will be displayed in the Treeview. If the analysis fails... In the event of the analysis failing due to errors in the model that you cannot correct, a file is provided to re-create all modelling features and attributes to allow the analysis to be run successfully. 94 Viewing the Results : Nonlinear Material lug_nonlinear_modelling.vbs example. File New… carries out the modelling of the Start a new model file. If an existing model is open Modeller will prompt for unsaved data to be saved before opening the new file. • Enter the file name as lug_nonlinear File Script Run Script... File LUSAS Datafile... > To recreate the model, select the file lug_nonlinear_modelling.vbs located in the \\Examples\Modeller directory. Rerun the analysis to generate the results. Viewing the Results : Nonlinear Material If the analysis was run from within LUSAS Modeller the results will be loaded on top of the current model and the load case results for load increment 1 are set to be active by default. Making the Pin invisible Note. When a results file is loaded on top of a corresponding model file groups of features can be made visible or invisible. This is of particular use when results are to be displayed only on selected parts of the model. In this example, results are only to be viewed on the Lug. Treeview right-click on the group name Lug and select the Set as Only • In the Visible option. Deformed Mesh Plot • With no features selected, click the right-hand mouse button in a blank part of the graphics window and de-select the Geometry option to remove the geometry Treeview. layer from the • If displayed, remove the Mesh and Attributes layers from the similar manner. Treeview in a • With no features selected, click the right-hand mouse button in a blank part of the Graphics window and select the Deformed mesh option to add the deformed Treeview. mesh layer to the • Click the OK button to accept the default mesh properties. 95 Contact Analysis of a Lug The deformed mesh plot will be displayed. Equivalent Stress Contour Plots • With no features selected click the right-hand mouse button in a blank part of the graphics window and select the Contours option to add the contours layer to the Treeview. The contour properties will be displayed. • Select Stress - Plane Stress contour results of Equivalent stresses SE • Click the OK button to display contours and a contour summary for the first load increment. • Change the layer display order to display the Deformed mesh on top of the Contours by selecting Deformed Mesh in the Treeview with the righthand mouse button and selecting the Move Down option. Changing the Active Results Loadcase • In the Treeview right-click on the last increment for load factor 2 and select the Set Active option. The contour plot for the final increment will be displayed. Note. Results for the other increments may be viewed simply by changing the active load case. Creating Animations As an alternative to viewing results individually for each load case, the change of stress due to the increasing load increments can be animated instead. To ensure 96 Viewing the Results : Nonlinear Material consistent contour values throughout the animation the range of contours is to be specified. For the final load increment the contour key shows a maximum stress in the order of 6.8E9. To create contours of 5E8 intervals the contour interval needs to be set. Treeview double-click on Contours. The contour layer properties will • In the be displayed. • Select the Contour Display tab and deselect the Contour key option. • Select the Contour Range tab and click the Interval button. Set the contour interval as 5E8. Click the Set as global range button and ensure that the Use global range button is also selected. • Click the OK button to finish. Note. When animating nonlinear loadcases it is important that the deformed mesh is plotted using a factor of 1 and not using a fixed screen size otherwise the deformed mesh for each load increment would be drawn the same. With this in mind: Treeview double-click on the Deformed mesh layer, select the Specify • In the Factor option, enter a factor to 1 and click OK Utilities Animation Wizard... • Select the Load history option and click the Next button. • Select lug_nonlinear.mys from the drop-down menu. The list of available load cases for selection will appear. Select the All loadcases button and the Finish button to create an animation for all loadcases and display the animation in a new window. Note. The buttons at the bottom of the window may be used to slow-down, speed-up, pause, step through frame by frame, or stop the animation. 97 Contact Analysis of a Lug Saving Animations Animations may be saved for replay in other standard windows animation players. • Ensure the animation window is the active window. File Save As AVI... • Enter lug_nonlinear for the animation file name. An .avi file extension is automatically appended to the file name when the file is saved. • Animations can be compressed to save disk space. A number of compression formats are available depending on what is installed on the system. Microsoft Video 1 has been found to provide reliable results. Click OK • Delete the animation window maximise the graphics window. and • Delete the Annotation layer from the Treeview. Creating Graphs Any set of results may be graphed against any other set of results. For example, a graph of resultant displacement for the node at the bottom of the hole of the lug is to be plotted against the load increment. • Select the node defining the bottom of the hole in the lug. Utilities Graph Wizard... The graph wizard provides a step-by-step means of selecting which results are to be plotted on the X and Y axes of the graph. The X axis is always defined first. Select this Node • Ensure the Time history option is selected and click the Next button. • Ensure the Nodal results button is selected and click the Next button. • Select Displacement results for resultant displacement RSLT. The node number of the previously selected node will be shown in the Specify node pull-down. Click the Next button. 98 Viewing the Results : Nonlinear Material The X axis results have been selected. The Y axis results to be graphed are now defined. • Select Named results and click the Next button. • Select Total Load Factor data. Click the Next button. Title information for the graph can be added at this stage. • Leave all title information blank. • Click the Finish button A graph is created in a new window with the values used shown in an adjacent table. To see the graph at the best resolution enlarge the window to a full size view. Note. The graph shows a linear displacement history for the node. This is because no geometric nonlinearity has been allowed for in the analysis. • Close the graph using the in the top right-hand corner of the graph window. Slideline Results Results can be presented on the contact surfaces as vectors or values, or as a graph on any specified load increment. • In the Treeview remove the Contours and Deformed mesh layers by selecting each in turn and clicking on the toolbar button. • With no features selected, click the right-hand mouse button in a blank part of the graphics window and select Mesh. Click OK to accept the default mesh properties. • In the Treeview select the slideline results group on which the results are to be displayed by right-clicking on the group Lug_Pin (master) and selecting the Set as Only Visible option. Click Yes to act on sub groups. 99 Contact Analysis of a Lug • In the Treeview ensure that the last load increment showing Load Factor = 2.00000 is active. • With no features selected, click the right-hand mouse button in a blank part of the graphics window and select the Values entry. • In the properties box, select the Entity Slideline Results and the Type ContPress to look at results of Contact Pressure. • Select the Values Display tab and de-select Symbols, ensure both Maxima and Minima are selected, set the range to 100 % and change the number of significant figures to 3. Click the OK button. To plot a graph of the contact pressure distribution around the contact surface: Utilities Graph Wizard... • Choose the Slidelines (assigned to lines) option and click Next • Select the Component ContPress • To plot the results against angle rather than length select the Calculate distance as angle option. • Click Next followed by Finish 100 Viewing the Results : Nonlinear Material Note. The graph properties and titles may be modified using the right-hand mouse button in the graph window if required. This completes the nonlinear analysis part of the example. 101 Contact Analysis of a Lug 102 Description Linear Buckling Analysis of a Flat Plate For software product(s): With product option(s): All. None. Description This example determines the critical buckling load for a 2m x 0.5m rectangular panel of 1mm thickness subject to in-plane compressive loading. Material properties for the panel are: Young's modulus 70E9 N/m2, Poisson's ratio 0.3. The panel is meshed using 64 Semiloof shell elements and is simply supported on all sides. An in-plane compressive load of a total of 24N is applied to one of the short edges, parallel to the long sides. Units used are N, m, kg, s, C throughout. Keywords 2D, Plate, Linear Buckling, Eigenvalue Buckling, Deformed Mesh, Printing 103 Linear Buckling Analysis of a Flat Plate Associated Files plate_modelling.vbs carries out the modelling of the example. Modelling Running LUSAS Modeller For details of how to run LUSAS Modeller see the heading Running LUSAS Modeller in the Examples Manual Introduction. Note. This example is written assuming a new LUSAS Modeller session has been started. If continuing from an existing Modeller session select the menu command File>New to start a new model file. Modeller will prompt for any unsaved data and display the New Model dialog. Creating a new model • Enter the file name as plate • Use the Default working folder. • Enter the title as Buckling of a flat plate • Set the units to N,m,kg,s,C • Select the model template Standard • Ensure the Structural user interface is selected. • Select the Vertical Z axis option. • Click the OK button. Note. Save the model regularly as the example progresses. Use the Undo button to correct any mistakes made since the last save was done. 104 Modelling Feature Geometry Geometry Surface Coordinates... > Enter coordinates of (0, 0), (2, 0), (2, 0.5) and (0, 0.5) to define a Surface. • Click the OK button. Meshing Attributes Mesh Surface… > • Select Thin shell, Quadrilateral, elements with Quadratic interpolation. • Enter the attribute name as Thin Shell. • Click the OK button. LUSAS will add the mesh dataset to the Treeview. • Select the Surface of the plate. • Drag and drop the Surface mesh attribute Thin Shell from the Treeview onto the selected feature. Note. If the number of divisions is not specified on the mesh dialog the default number of 4 divisions per Line will be used. In this example 4 divisions per Line is sufficient for the ends of the plate but 16 divisions are required on each of the sides. • In the Treeview double-click on the Line mesh Divisions=8 • On the Line Mesh dialog change the number of line divisions to 16, change the Attribute name to Divisions=16 and click the OK button. • Select the two long sides of the plate and drag and drop the Line mesh attribute Divisions=16 from the Treeview onto the selected features. 105 Linear Buckling Analysis of a Flat Plate Geometric Properties Attributes Geometric Surface... > • Specify a thickness of 0.001. • Enter the attribute name as Plate Thickness (The eccentricity can be left blank, as it is not used in this analysis). • Click the OK button to add the attribute to the Treeview. • With the Surface selected, drag and drop the geometry attribute Plate Thickness from the Treeview onto the selected feature. Assigned geometric attributes are visualised by default. Select the fleshing on/off button to turn-off geometric property visualisation. Material Properties Attributes Material Isotropic… > • Specify the Young's modulus as 70E9 • Enter Poisson's ratio as 0.3 (Mass density can be left unspecified for Eigenvalue buckling analyses). • Enter the attribute name as Plate Material • Click the OK button to add the attribute to the Treeview. • With the Surface selected, drag and drop the material attribute Plate Material from the Treeview onto the selected surface. Supports LUSAS provides the more common types of support by default. These can be seen in the Treeview. Four support datasets are to be assigned to selected features of the model. 106 Modelling • Select the top line, hold the Shift key, and select the left and bottom Lines as shown. • Drag and drop the Fixed in Z support attribute from the Treeview onto the selected Lines. Lines 'Fixed in Z' Points 'Fixed in YZ' Line 'Fixed in XZ' Point 'Fully Fixed' • Ensure that the supports are assigned to Lines for All loadcases and click the OK button. • Similarly for each of the other features shown above drag and drop the relevant support attributes from the Treeview to assign the required supports. Use the Isometric button to rotate the model to this view. • Check the position and type of supports on the model match those above. Loading A global distributed load is to be applied to the lefthand end of the plate. 107 Linear Buckling Analysis of a Flat Plate Attributes Loading... • Select the Global Distributed option and click Next • Enter a Total load of 24 in the X direction. • Enter the attribute name as Distributed Load. • Click the button. Finish • Select the left hand edge of the plate and drag and drop the loading dataset Distributed Load from the Treeview onto the selected Line. • Click OK to assign the load to Loadcase 1 with a factor of 1 Eigenvalue Analysis Control Eigenvalue analysis control is defined as a loadcase property. • In the Treeview right-click on Loadcase 1 and select Eigenvalue from the Controls menu. • Select a Buckling Load solution for the Minimum number of eigenvalues. 108 Running the Analysis • Enter the Number of eigenvalues required as 3 • Enter the Shift to be applied as 0 • Click the OK button to select the Default eigensolver. Saving the model File Save Save the model file. Running the Analysis File LUSAS Datafile... A LUSAS data file name of plate will be automatically entered in the File name field. • Ensure that the options Solve now and Load results are selected. • Click the Save button to solve the problem. A LUSAS Datafile will be created from the model information. The LUSAS Solver uses this datafile to perform the analysis. If the analysis is successful... Eigenvalue results files will be seen in the Treeview. In addition, 2 files will be created in the directory where the model file resides: plate.out this output file contains details of model data, assigned attributes and selected statistics of the analysis. plate.mys this is the LUSAS results file which is loaded automatically into the Treeview to allow results processing to take place. If the analysis fails... If the analysis fails, information relating to the nature of the error encountered can be written to an output file in addition to the text output window. Select No to not view the output file. Any errors listed in the text output window should be corrected in LUSAS Modeller before saving the model and re-running the analysis. 109 Linear Buckling Analysis of a Flat Plate Rebuilding a Model If it proves impossible for you to correct the errors reported a command file is provided to enable you to re-create the model from scratch and run an analysis successfully. plate_modelling.vbs carries out the modelling of the example. File New… Start a new model file. If an existing model is open Modeller will prompt for unsaved data to be saved before opening the new file. • Enter the file name as plate File Script Run Script... File LUSAS Datafile... > • To recreate the model, select the file plate_modelling.vbs located in the \\Examples\Modeller directory. Rerun the analysis to generate the results. Viewing the Results If the analysis was run from within LUSAS Modeller the results will be loaded on top of the current model and the loadcase results for each eigenvalue can be seen in the Treeview. • Delete the Mesh, Geometry and Attributes layers from the Treeview. Deformed Mesh Plot • With no features selected, click the right-hand mouse button in a blank part of the Graphics window and select the Deformed mesh option to add the deformed mesh layer Treeview with a to the magnitude of 6. Click the OK button to display the first eigenmode shape. Use the Dynamic Rotation button to ensure that the model is rotated to a similar view to that shown. 110 Viewing the Results Return to normal cursor mode Changing the Results Loadcase To view the second eigenmode: • In the Treeview right-click on Eigenvalue 2 and select the Set Active option. The second eigenmode shape will be displayed. The third eigenmode can be viewed in a similar manner. Note. Mode shapes may be the opposite those shown. Printing the Buckling Load Factors • In an eigenvalue buckling analysis, the load factors are equivalent to the eigenvalues. Load factors are the values by which the applied load is factored to cause buckling in the respective modes. Eigenvalue results for the whole model can be displayed in the text window. Utilities Print results wizard... • Select the entity None and ensure that results type Eigenvalues is selected and click the Finish button. The Eigenvalue results will be printed to the text window with the Load factors being given in the eigenvalue results column Note that error norms may vary from those shown. 111 Linear Buckling Analysis of a Flat Plate Calculating the Critical Buckling Load The applied load (24N) must be multiplied by the first load factor (19.0779) to give the value of loading which causes buckling in the first mode shape. The initial buckling load is therefore 24x19.0779 = 457.87 N. Note. An applied load of unity could be used in an eigenvalue analysis - in which case the eigenvalues produced would also represent the critical loads at which the structure would buckle. However, to prevent potential convergence problems with the analysis it is more usual to apply actual in-service loading and multiply the applied load by the eigenvalue to give the critical buckling load for each eigenvalue. This completes the example. 112 Description Elasto-Plastic Analysis of a VNotch For software product(s): With product option(s): All. Nonlinear. Description A 5mm thick Vshaped, notched specimen is to be subjected to two load types; a pressure load distributed along the inner edge of its opening and a loading caused by pushing a bolt into the notch of the specimen. 90 10 30 Centreline Radius 10 40 All dimensions in mm After an initial linear analysis with the specimen subjected to the pressure load, nonlinear material properties are defined and a nonlinear analysis is carried out using the same pressure loading. An additional linear and nonlinear analysis is done to investigate the insertion of a bolt into the notch of the specimen with slidelines being used to model the contact behaviour between the two components. Because of symmetry only half of the Vnotch need be modelled. Units are N, mm, t, s, C throughout. 113 Elasto-Plastic Analysis of a V-Notch Objectives Initial Yield Investigate the load which causes initial yielding. Spread of Yield Under continued loading investigate the progression of plastic deformation under pressure loading. Ultimate Capacity (Pressure) Investigate the ultimate capacity of the specimen under pressure loading. Transfer of Force from Bolt Investigate the transfer of forces from the loading bolt from a preliminary linear contact and subsequent nonlinear contact analysis. Keywords Plane Stress, Contact, Geometrically Nonlinear (GNL), Materially Nonlinear (MNL), Contour Plot, Elasto-Plastic, Yield, Yield Symbol, Plastic Strain, Animation Associated Files vnotch_linear_modelling.vbs carries out the modelling for the linear notch analysis. vnotch_nonlinear_modelling.vbs carries out the modelling of the nonlinear material model. vnotch_linear_contact_modelling.vbs carries out the modelling of the specimen using a linear analysis and a geometrically nonlinear model. vnotch_nonlinear_contact_modelling.vbs carries modelling of the notch and bolt with nonlinear material properties. out the Discussion The response of this component is dominated by materially nonlinear effects. After an initially elastic response, the material undergoes elastic-plastic yielding. In a simple von Mises model the tensile and compressive stress regions are considered to cause identical plasticity. The post-yield response is governed by the hardening slope. A zero slope denotes elastic-perfectly plastic behaviour. Analysis 1. Linear Material Analysis An initial linear investigation is performed to verify the model and to find the maximum stress induced by a unit intensity load. This information is used to design the incrementation strategy for the initial coarse nonlinear analysis. 114 Modelling : Linear Material Analysis 2. Nonlinear Material Analysis The material nonlinearity is specified in LUSAS by the addition of plastic material properties and a hardening curve. The nonlinear strategy is designed such that the first increment (arrived at from the linear analysis) stresses the material to just below yield in a single step. The model is loaded until a specified displacement is reached at a selected Point. The incrementation strategy is designed to develop the yielded region in a gradual and stable manner. Analysis 3. Contact Analysis with Linear Materials Once the behaviour of the structure is understood under pressure-loaded conditions, the pressure load is removed. A bolt is added to the model and slidelines are defined to model the contact between the notch and the bolt. Analysis 4. Contact Analysis with Nonlinear Materials Once the behaviour of the multiple-bodied structure is understood the nonlinear materials in the specimen are re-introduced and a full geometric, nonlinear contact analysis performed. Modelling : Linear Material This worked example will create a LUSAS model of half of the notched V-specimen. Initially, a linear elastic analysis with an applied unit structural face load will be prepared. Then the material properties will be made nonlinear and a suitable analysis control defined and assigned. Running LUSAS Modeller For details of how to run LUSAS Modeller see the heading Running LUSAS Modeller in the Examples Manual Introduction. Note. This example is written assuming a new LUSAS Modeller session has been started. If continuing from an existing Modeller session select the menu command File>New to start a new model file. Modeller will prompt for any unsaved data and display the New Model dialog. Creating a new model • Enter the file name as vnotch_linear • Use the Default working folder. 115 Elasto-Plastic Analysis of a V-Notch • Enter the title as V-Notch - Linear Analysis • Select the units N,mm,t,s,C • Select the model template Standard from those available in the drop down list. • Ensure the Structural user interface is being used. • Select the Vertical Y axis option and click OK Note. Save the model regularly as the example progresses. Use the Undo button to correct any mistakes made since the last save was done. Feature Geometry Geometry Line Coordinates... > Using the X and Y coordinates shown in the table define Points which mark out half of the model. Use the Tab key to move to the next entry field. Use the arrow keys to move around fields. • Click the OK button to finish. X 90 90 0 0 30 Y 20 30 30 0 0 Note. The Z coordinate does not have to be entered. A dimension of zero will be assumed. The V shaped notch will be created using an arc and a Line drawn tangential to the arc. • Select the Point shown to generate the arc. Geometry Line > Arc/Circle > By Sweeping Points… Select this Point Rotate the Point through an angle of -120 degrees about an origin of (40,0). Click the OK button to finish. 116 Modelling : Linear Material • Select the Point shown and add the Arc to the selection by holding down the Shift key. Select this Point Select this Line Geometry Line Tangent Point to Line > > • Ensure that Split tangent line and Delete geometry on splitting are selected on the Tangent dialog. • Click OK to draw the Line representing the notch. The model can now be tidied by zooming in on a region of the model around the arc and deleting the redundant Lines and Points. • Drag a box to select the features shown. Delete the selected features, confirming that Lines and Points are to be deleted. Resize the view to show the whole model. Drag a box to select these features Note. Points and Lines used to define features extending outside of the area selected will not be deleted. Finally, a Surface is to be created from the line features. • Select the whole model using the Ctrl and A keys together. Geometry Surface Lines... > Create a General Surface from the selected Lines. 117 Elasto-Plastic Analysis of a V-Notch Meshing Attributes Mesh Surface… > • Define Plane stress, Triangle, Quadratic elements with an Irregular mesh spacing. Ensure that a specified element size is not selected. • Enter the mesh attribute name as Plane Stress TPM6 and click OK LUSAS will add the mesh attribute to the Treeview. • Select the newly created surface using the Ctrl and A keys together. • Drag and drop the Surface mesh attribute Plane Stress TPM6 Treeview from the onto the selected features. Click OK to complete the mesh assignment. Note. TPM6 elements are low-order elements and are used in this example to keep within the evaluation version limits. More accurate modelling is obtained when using Plane Stress, Quadrilateral, Quadratic elements (QPM8) which have more nodes per element. LUSAS will mesh the Surface based upon a default Line division of 4. To improve the shape and arrangement of elements, Line mesh attribute will be used to control the Surface mesh density. Attributes Mesh Line... > • With the Element description set as None, define an average Element length of 5 mm. Enter the Line mesh attribute name as Element Length 5 and click OK • With the whole model selected, drag and drop the Line mesh attribute Element Length 5 from Treeview onto the the selected features. The mesh arrangement will be displayed. Local mesh refinement will now be applied by giving the Arc a finer Line mesh. Attributes Mesh Line… > • Define an average Element length of 2.5 mm. • Enter the Line mesh attribute name as Element Length 2.5 and click OK 118 Modelling : Linear Material • Select the arc • Drag and drop the Line mesh attribute Element Length 2.5 from the Treeview onto the selected Line. The mesh will be refined as shown. Geometric Properties Attributes Geometric Surface… > • Define a geometric property attribute with a thickness of 5 mm. • Enter the attribute name as Thickness=5 and click OK to add the attribute to the Treeview. • With the whole model selected, drag and drop the geometry attribute Thickness=5 from the Treeview onto the selected features. Select the fleshing on/off button to turn-off the automatic geometric property visualisation. Material Properties The only material properties that are essential for a linear elastic static analysis are Young's modulus and Poisson's Ratio. The units of Young's modulus in this particular example are N/mm2. Attributes Material Isotropic… > • With the Elastic tab selected, enter a Young's modulus of 210e3 and a Poisson's Ratio of 0.3. Leave the other fields blank. • Enter the attribute name as Steel (N mm)and click OK to add the attribute to the Treeview. • With the whole model selected, drag and drop the material attribute Steel (N mm) from the Treeview onto the selected features and click OK to assign to surfaces. Support Conditions LUSAS provides the more common types of support by default. These can be seen in the Treeview. The specimen is to be restrained along the horizontal axis of symmetry in the X and Y axes. 119 Elasto-Plastic Analysis of a V-Notch • Select the horizontal Line along the axis of symmetry. • Drag and drop the support attribute Fixed in XY from Treeview the onto the selected Line and click OK to assign to lines. Select this Line Loading A unit pressure load is to be defined and applied to the edge of the Surface Attributes Loading… • Select the Face option and click Next • Define a face load in the y direction of 1 • Enter the attribute name as Face Load 1 and click Finish Note. Face loads are pressure loads which can be applied to the edges of Surfaces or the faces of Volumes. • Select the angled Line of the notch. • Drag and drop the loading attribute Face Load 1 from Treeview onto the the selected Line and click OK to assigned to Lines. Note. Structural face loading uses local element directions. If the loading is incorrectly oriented it may be due to the local element direction of the Surface. To rectify this either reverse the element direction of the Surface by selecting the Surface using Geometry> Surface> Reverse or double-click on the loading attribute name in the Treeview and change the sign of the loading. 120 Running the Analysis : Linear Material Saving the model File Save Save the model file. Running the Analysis : Linear Material File LUSAS Datafile… A LUSAS data file name of vnotch_linear will be automatically entered in the File name field. • Ensure that the options Solve now and Load results are selected. • Click the Save button to finish. A LUSAS Datafile will be created from the model information. The LUSAS Solver uses this datafile to perform the analysis. If the analysis is successful... The LUSAS results file will be added to loadcase section of the Treeview. In addition, 2 files will be created in the directory where the model file resides: vnotch_linear.out this output file contains details of model data, assigned attributes and selected statistics of the analysis. vnotch_linear.mys this is the LUSAS results file which is loaded automatically into the Treeview to allow results processing to take place. If the analysis fails... If the analysis fails, information relating to the nature of the error encountered can be written to an output file in addition to the text output window. Any errors listed in the text output window should be corrected in LUSAS Modeller before saving the model and re-running the analysis. Rebuilding a Model If it proves impossible for you to correct the errors reported a file is provided to enable you to re-create the model from scratch and run an analysis successfully. vnotch_linear_modelling.vbs carries out the modelling of the example. 121 Elasto-Plastic Analysis of a V-Notch File New… Start a new model file. If an existing model is open Modeller will prompt for unsaved data to be saved before opening the new file. • Enter the file name as vnotch_linear File Script Run Script... File LUSAS Datafile... > To recreate the model, select the file vnotch_linear_modelling.vbs located in the \\Examples\Modeller directory. Rerun the analysis to generate the results Viewing the Results : Linear Material If the analysis was run from within LUSAS Modeller the results will be loaded on top of the current model and the loadcase results will be seen in the Treeview. Deformed Mesh Plot Once the linear version of the model has been run it is prudent to check the deformed shape for obvious errors such as overlarge displacements in unexpected areas, which could be accounted for by incorrect properties, incorrect positioning of the load or incorrect support conditions. The deformed shape also provides a general check on the overall load direction. • If present in the Treeview delete the Mesh, Geometry and Attributes layers. • With no features selected click the right-hand mouse button in a blank part of the Graphics window and select the Deformed mesh option to add the deformed mesh layer to the Treeview. • Click the OK button to display the deformed mesh plot. 122 Viewing the Results : Linear Material Von Mises Stress Contours The linear elastic results provide an opportunity to establish a faster loading scheme for the nonlinear analysis to come. Checking the maximum von Mises stress values will allow calculation of a factor of load that can be sustained without yielding the material. • With no features selected click the right-hand mouse button in a blank part of the Graphics window and select the Contours option to add the contour layer to the Treeview. • Select entity Stress and Plane Stress component equivalent stress SE • Click the OK button to display the contours. Changing the layer display order Note. The order of the layer names in the Treeview determines the order in which the layers will be displayed. To make a layer display after another layer, click Treeview and drag the layer name onto the layer name on the layer name in the after which it is to be displayed. The display in the graphics window will be updated accordingly. • Following the note above make the deformed mesh display after the contours by dragging the Deformed Mesh layer onto Contours layer in the Treeview. Note. The material chosen for the analysis is assumed to yield at 300 N/mm2. From the contour key results the maximum stress induced from a unit face load results in a stress of just over 30 N/mm2. Therefore, a factored load value of 9 would be suitable for use as the first load increment level in the nonlinear analysis as this would result in stresses just below the yield stress. 123 Elasto-Plastic Analysis of a V-Notch Modelling : Nonlinear Material Files. The geometry of the notch is the same as that defined for the linear model. It may be recovered by one of two methods. File Open... If the previous linear analysis was performed successfully open the model file vnotch_linear.mdl which was saved after completing the first part of this example and select No to not load a results file of the same name on top of this model. File Save As... • Enter the model file name as vnotch_nonlinear and click the Save button. Creating the starting model from a supplied file File New… Alternatively, start a new model file. If an existing model is open Modeller will prompt for unsaved data to be saved before opening the new file. • Enter the file name as vnotch_nonlinear File Script Run Script... > To create the model, select the file vnotch_linear_modelling.vbs located in the \\Examples\Modeller directory. Change the model description File Model Properties… Change the model description to V-Notch - Nonlinear Analysis and click OK Modifying the Material The linear material dataset needs to be modified to include plastic properties. • In the Treeview double-click on the material attribute Steel (N mm) • Select the Plastic check box and for a Stress potential model enter an Initial uniaxial yield stress of 300 • Select the Hardening check box, select the Hardening gradient option and enter a Slope of 0 and a Plastic strain of 1000 in the first row of the table. • Click the OK button to finish and overwrite the existing material dataset. Note. The von Mises material model used assumes identical behaviour in compression and tension. 124 Modelling : Nonlinear Material Nonlinear Analysis Control From the results of the Linear analysis, initial yielding is expected at a load factor of nearly 10 (Yield Stress/Max Stress). Therefore the nonlinear loading strategy will be to apply an initial load factor of 9, and use unit factor increments as the yielding progresses. The analysis will be set to stop once the Point at the inside end of the arm of the notch has displaced 10mm from its original position. • Ensure that the geometry layer is displayed. If necessary, with no features selected click the right-hand mouse button in a blank part of the graphics window and Treeview. select the Geometry option to add the geometry layer to the • Select the Point at the end of the notch as shown. Note. The number of the Point selected will be displayed in the status bar at the bottom of the graphics window. Select this Point Analysis control options are defined as loadcase properties. Treeview right-click on Loadcase 1 and select Nonlinear and • In the Transient from the Controls menu. The Nonlinear & Transient dialog will appear. • Select the Nonlinear option. • From the Incrementation drop down list select Automatic control. • Set the Starting load factor as 9 • Set the Max change in load factor as 1 • Set the Max total load factor as 0 to enable the load to increase without limit. The dialog should appear as shown: 125 Elasto-Plastic Analysis of a V-Notch To terminate the load on a limiting variable the advanced nonlinear parameters need to be set in the Incrementation section. • Select the Incrementation Advanced button. • Click the Terminate on value of limiting variable option. • Set the Point number from the drop-down list to the Point selected earlier. • Set the Variable type in the drop down list as V to limit the displacement in the local Y direction. • Set the Value as 10 • Click the Allow step reduction option. 126 Running the Analysis : Nonlinear Material The dialog should appear as shown below. • Click the OK button to return to the load case dialog. • Click the OK button to finish. Save the model File Save To save the model. Note Geometric stiffening is not considered in this example because the nonlinear effects are predominantly due to yield in the material. Running the Analysis : Nonlinear Material File LUSAS Datafile… A LUSAS data file name of vnotch_nonlinear will be automatically entered in the File name field. • Ensure that the options Solve now and Load results are selected. • Click the Save button to finish. A LUSAS Datafile will be created from the model information. The LUSAS Solver uses this datafile to perform the analysis. 127 Elasto-Plastic Analysis of a V-Notch During the analysis… Apart from the increment and iteration, several parameters output are of special interest during the nonlinear analysis phase: TLMDA (Total Load Factor) The factor of load applied using the incrementation control is displayed here. It shows how the load application is progressing for a load control and an arc-length solution. DTNRM (Displacement Norm) The changes in this value indicate how well the problem is converging. If the analysis is successful... The LUSAS results file will be added to the Treeview. In addition, 2 files will be created in the directory where the model file resides: vnotch_nonlinear.out this output file contains details of model data, assigned attributes and selected statistics of the analysis. vnotch_nonlinear.mys this is the LUSAS results file which is loaded automatically into the Treeview to allow results processing to take place. If the analysis fails... If errors are listed that for some reason you cannot correct, a file is provided to recreate the model information correctly, allowing a subsequent analysis to be run successfully. vnotch_nonlinear_modelling.vbs carries out the complete nonlinear material modelling of the example. File New… Start a new model file. If an existing model is open Modeller will prompt for unsaved data to be saved before opening the new file. • Enter the file name as vnotch_nonlinear File Script Run Script... File LUSAS Datafile... > To re-create the model, select the file vnotch_nonlinear_modelling.vbs located in the \\Examples\Modeller directory. Rerun the analysis to generate the results 128 Viewing the Results : Nonlinear Material Viewing the Results : Nonlinear Material This section covers a typical results processing session for a nonlinear analysis. In this session the following procedures will be carried out: A von Mises stress contour plot and associated yielded region plot will be drawn. A graph showing the displacement history of the notch opening through the analysis will be created. If the analysis was run from within LUSAS Modeller the results will be loaded on top of the current model and the load case results for loading increment 1 will be set active by default. Plotting Stress Contours • Delete all layers from the Treeview. • Click the right-hand mouse button in a blank part of the graphics window and select Contours. • On the contour property dialog. select entity Stress - Plane Stress and component equivalent stress SE • Click the Contour Range tab and set the Maximum stress contour value to be plotted as 300 so all stresses above yield are drawn in red. • Click the OK button to display contours for the first load increment. • With no features selected click the right hand mouse button in a blank part of the graphics window and select the Mesh layer. • Select OK to accept the default properties and add the mesh to the display. The display will show that the yield stress of 300Nmm-2 has not been reached after the first loading increment. 129 Elasto-Plastic Analysis of a V-Notch Changing the Active Results Loadcase • In the Treeview, rightclick on the last load increment and select the Set Active option. Contours for the selected increment will be displayed.. The red area shows the peak von Mises stress which is being limited to 300 N/mm2 by the zero hardening slope as defined in the plastic material properties section for the model. Yielded Material Plot In addition to using contours to show yielded regions of the model, the spread of plasticity can be visualised using yield symbols. • With no features selected click the right hand mouse button in a blank part of the graphics window and select the Values layer. • Select the Stress - Plane Stress entity and Yield component and click the OK button to display the yielded Gauss points with an asterisk. • Select No to not change the contour layer to match. Note. By changing the active loadcase the spread of yield through the model can be viewed. 130 Viewing the Results : Nonlinear Material Displacement History Graph To illustrate the nonlinear behaviour of the model a displacement history graph showing the displacement of a node on the notch against the total applied load factor is to be displayed. • Select the node on the end of the notch as shown. Select this Node The graph wizard provides a step-by-step means of selecting which results are to be plotted on the X and Y axes of the graph. The X axis is always defined first. Utilities Graph Wizard… • Ensure the Time history option is selected and click the Next button. • Ensure the Nodal results button is selected for the X axis results and click the Next button. • Select Displacement from the entity drop down list for the component DY. The node number of the selected node will be shown. Click the Next button. This defines the X axis results. • Select Named results and click the Next button. • From the drop down list select Total Load Factor data and click the Next button. 131 Elasto-Plastic Analysis of a V-Notch This defines the Y axis results. • Leave all title and axis fields blank and click the Finish button to create the graph in a new window and display the values used in an adjacent table. To see the graph at the best resolution enlarge the window to a full size view. Note. The graph shows the progressive softening of the structural response as the load is increased. The load value corresponding to the flat section represents the limit of the load carrying capacity of the model. Delete the graph window. Modelling : Contact Analysis (Linear Material) This section details the changes required to the linear material model from the first part of the example to incorporate the geometry of a bolt which will be positioned and loaded to prise the notch arms apart. File Open... If the initial linear analysis was performed successfully open the model file vnotch_linear.mdl saved after completing the first part of this example and select No to not load a results file of the same name on top of this model. File Save As... • Enter the model file name as vnotch_contact and click the Save button. Creating the starting model from a supplied file File New… Alternatively, start a new model file. If an existing model is open Modeller will prompt for unsaved data to be saved before opening the new file. • Enter the file name as vnotch_linear_contact File Script Run Script... > To create the model, select the file vnotch_linear_modelling.vbs located in the \\Examples\Modeller directory. 132 Modelling : Contact Analysis (Linear Material) • Change the model description to V-Notch - Contact Analysis (Linear Material) and click OK File Model Properties… Deassigning the Loading The initial pressure loading is no longer required. In the nonlinear contact model the loading will be applied as a prescribed displacement to the centre-line of the bolt. Treeview click the right hand mouse button on the loading attribute • In the Face Load 1 and select the Deassign > From all option. Modelling the Bolt Note. At this stage the bolt will be defined separated from the notch specimen. This will make assigning the attributes, especially the slidelines, easier. Once the attributes are assigned, the bolt will be moved to its starting position before the analysis is run. • Ensure the Geometry layer is present in the Geometry Line Coordinates... > Treeview. Enter coordinates of (75,0), (90,0) and (105,0) and click OK to define 2 horizontal Lines on the bolt centreline. Enter coordinates of (90,0) and (90,15) and click OK to define a vertical Line on the bolt centreline. An arc is to be drawn to form the upper half of the bolt. • Select the 3 Points in the order shown. Geometry Line > Arc/Circle From Coords/Points … 2. Select this Point • Click OK to accept the values present on the dialog and the arc will be drawn. 1. Select this Point 3. Select this Point This arc will now be split into 2 new arcs. • Select the arc just drawn 133 Elasto-Plastic Analysis of a V-Notch Geometry Line By splitting In Equal Divisions… Geometry Surface Lines… > > • Enter the number of divisions as 2 • Click OK to create 2 arcs and delete the original arc. • Select the left hand arc and then the 2 Lines as shown. > 1. Select this Arc The left hand Surface of the bolt will be drawn. 2. Select this Line • Select the right-hand arc and then the other 2 Lines to create the Surface for the other half of the bolt. Geometry Surface Lines… > 3. Select this Line The right-hand Surface of the bolt will be drawn. Meshing the Bolt • In the Treeview double-click on the mesh attribute Plane Stress TPM6 • Change the element shape to Quadrilateral, select Regular Mesh, and change the attribute name to Plane Stress Quads. • Click the OK button to create a new mesh dataset in the • Select both Surfaces defining the bolt and drag and drop the surface mesh dataset Plane Stress Quads from the Treeview onto the selected features. Treeview. Select these 2 Surfaces 134 Modelling : Contact Analysis (Linear Material) Modifying the mesh on the bolt • Select the 2 arcs at the top of the bolt as shown. Select these 2 Lines for 'Divisions = 6' • Drag and drop the line mesh attribute Divisions=6 from Treeview the onto the selected Lines. The mesh will be redrawn as shown. Geometric Properties • In the Treeview double click on the geometry attribute Thickness=5 • Change the thickness to 10 and change the attribute name to Thickness=10 • Click the OK button to create a new geometric mesh attribute in the Treeview. • Select both Surfaces of the bolt and drag and drop the geometry attribute Thickness=10 from the Treeview onto the selected features. Material Properties • With the bolt selected, drag and drop the material attribute Steel (N mm) from the Treeview onto the selected features. Note. At this stage the material model is linear elastic and does not include plasticity effects. The addition of plasticity is included at the next stage of the example. Support Conditions A roller support is required at the bolt centreline to restrain in the Y direction only. 135 Elasto-Plastic Analysis of a V-Notch • Select the 2 horizontal Lines on the bolt centreline. • Drag and drop the support attribute Fixed in Y from the Treeview onto the selected lines. • Click OK to assign the support dataset to the selected Lines. Loading Conditions An incremental prescribed displacement will be used. At this stage a negative unit displacement will be applied. The magnitude of each increment is controlled later using nonlinear control parameters. Attributes Loading… • Select the Prescribed Displacement option and click Next • Select the Incremental button and enter a prescribed displacement in the X direction of -1 • Enter the attribute name as Prescribed Load 1 and click Finish • With the 2 horizontal Lines on the bolt centreline selected, drag and drop the loading dataset Prescribed Load 1 from the Treeview onto the selected features. • Click OK to assign the loading to Loadcase 1 with a factor of 1 Slideline Definition Slidelines automatically model components having dissimilar meshing patterns and can also model any frictional contact between interacting components. Slidelines are to be applied to the contacting Lines of the notch and the bolt. 136 Modelling : Contact Analysis (Linear Material) Attributes Slideline… • Ensure the Master Stiffness Scale and Slave Stiffness Scale values are set to 1 and leave the remaining values as defaults. • Enter the slideline attribute name as Slideline 1 and click OK to add the slideline attribute to the Treeview. The Coulomb friction coefficient defaults to zero, which will define a standard no friction slideline. • Select the inclined Line of the notch. Select this Line for the Master • Drag and drop the slideline attribute Slideline 1 from Treeview the onto the selection. Select this Line for the Slave • Ensure the Master option is selected and click OK to accept the default orientation. • Select the left arc of the bolt. • Drag and drop the slideline attribute Slideline 1 from the selection. • Treeview onto the Select the Slave option and click the OK button to accept the default orientation. • To visualise the slidelines assigned to the model click the right-hand mouse button on the slideline attribute name in Treeview the and select Visualise MasterAssignments and Visualise Slave Assignments • Repeat the process above to deselect the slideline visualisation. All assignments are now complete, and the bolt can be moved into a starting position just adjacent to the notch ready for the analysis. • Drag a selection box around the bolt. 137 Elasto-Plastic Analysis of a V-Notch Geometry Point Move… > Enter a translation of -24 in the X direction. • Leave the attribute name blank and click the OK button to move the bolt into position. Nonlinear Analysis Control A bolt displacement of 1mm is to be specified. This will be done in 10, 0.1mm increments using nonlinear control properties. The nonlinear analysis control parameters are applied as properties of the loadcase. Treeview right-click on Loadcase 1 and select Nonlinear and • In the Transient from the Controls menu. The Nonlinear & Transient dialog will appear. • Set Nonlinear incrementation with Automatic control. • Set the Starting load factor as 0.1 • Set the Maximum change in load factor as 0.1 • Set the Maximum total load factor as 1 • Deselect the option to Adjust load based upon convergence • Click the OK button to finish the definition of the nonlinear parameters. Saving the model File Save To save the model. Running the Analysis : Contact Analysis (Linear Material) With the model loaded: File LUSAS Datafile… A LUSAS data file name of vnotch_linear_contact will be automatically entered in the Filename field. 138 Running the Analysis : Contact Analysis (Linear Material) • Ensure that the options Solve now and Load results are selected. • Click the Save button to finish. A LUSAS Datafile will be created from the model information. The LUSAS Solver uses this datafile to perform the analysis. If the analysis is successful... The LUSAS results file will be added to the Treeview. In addition, 2 files will be created in the directory where the model file resides: vnotch_linear_contact.out this output file contains details of model data, assigned attributes and selected statistics of the analysis. vnotch_linear_contact.mys this is the LUSAS results file which is loaded automatically into the Treeview to allow results processing to take place. If the analysis fails... If errors are listed that for some reason you cannot correct, a file is provided to recreate the model information correctly, allowing a subsequent analysis to be run successfully. vnotch_linear_contact_modelling.vbs carries out the modelling of the example. File New… Start a new model file. If an existing model is open Modeller will prompt for unsaved data to be saved before opening the new file. • Enter the file name as vnotch_linear_contact File Script Run Script... File LUSAS Datafile... > To recreate the model, select the file vnotch_linear_contact_modelling.vbs located in the \\Examples\Modeller directory. Rerun the analysis to generate the results 139 Elasto-Plastic Analysis of a V-Notch Viewing the Results - Contact Analysis (Linear Material) If the analysis was run from within LUSAS Modeller the results will be loaded on top of the current model and the loadcase results for each load increment can be seen in Treeview. The results for load increment 1 are set to be active by default. the Equivalent Stress Contour Plots If present in the Treeview delete the Mesh, Geometry and Attributes layers. • With no features selected click the right-hand mouse button in a blank part of the graphics window and select Deformed mesh to add the deformed mesh layer to Treeview. the • On the deformed mesh dialog, click the Specified factor option and enter a Factor of 1 and click the OK button. Note. When viewing results for contacting components it is important that the deformed mesh is plotted using a specified factor of 1 rather than a specified magnitude otherwise the components appear to contact incorrectly. • With no features selected click the right-hand mouse button in a blank part of the Graphics window and select the Contours option to add the contours layer to the Treeview and display the contour properties. • On the contour properties dialog select entity Stress - Plane Stress and component equivalent stress SE from the contour property dialog. • Click the Contour range tab and set the Maximum stress contour value to be plotted as 300 so all stresses above yield will be drawn in red. • Click the OK button to display the contours and contour key for the first load increment. • Change the layer display order to display the deformed mesh on top of the contour plot. The contour arrangement shows that the first load increment does not induce any stresses in the arms of the notch since contact has not yet taken place. 140 Modelling : Contact Analysis (Nonlinear Material) Changing the Active Results Loadcase • In the Treeview right-click on the last load increment for load factor 1.0 and select the Set Active option. The contour plot for the final increment will be displayed. From this stress plot where the bolt displacement is 1mm, it can be seen from the contour key that the material in the root of the notch is stressed to levels above the yield value of the material. Note. By investigating the other load increments it can be seen that after the third load increment the bolt begins to induce stresses in the notch and that the load is transferred from the bolt to the specimen via the slidelines. Modelling : Contact Analysis (Nonlinear Material) Creating the Model Files. The geometry of the notch lug is the same as that defined for the geometrically nonlinear contact analysis model. It may be recovered by one of two methods. File Open... If the linear contact analysis was performed successfully re-open the model file vnotch_linear_contact.mdl and select No to not load a results file of the same name on top of this model. File Save As... • Enter the model file name as vnotch_nonlinear_contact and click the Save button. Creating the starting model from a supplied file File New… Alternatively, start a new model file. If an existing model is open Modeller will prompt for unsaved data to be saved before opening the new file. • Enter the file name as vnotch_nonlinear_contact 141 Elasto-Plastic Analysis of a V-Notch File Script Run Script... > To create the model, select the file vnotch_linear contact.vbs located in the \\Examples\Modeller directory. Changing the model description File Model Properties… • Change the model description to V-Notch - Contact Analysis (Nonlinear Material) and click OK Modifying the Geometry The linear material attribute needs to be modified to include plastic properties. • In the Treeview double-click on the material attribute Steel (N mm) • Select the Plastic button and enter an Initial uniaxial yield stress of 300 • Select the Hardening button, select the Hardening gradient button and enter a Slope of 0 and a Plastic strain of 1000 in the first line of the table. • Click the OK button to overwrite the existing material definition. Note. The perfectly plastic assumption is an initial simplification that would in practice be replaced by a more detailed description of the hardening behaviour of the material. This would typically involve specifying several hardening gradients (i.e nonlinear hardening) and the strain limits to which each slope applies. Nonlinear Analysis Control The nonlinear control properties required for this section of the analysis are already specified in the current model. However, the bolt displacement of 1mm is to be increased to 2.5mm by specifying 25, 0.1mm increments in the nonlinear section of the load case dialog. Treeview double-click on Nonlinear and Transient to edit the existing • In the parameters. • Set the Max total load factor to 2.5 • Click the OK button to return to the graphics window. Save the model File Save Save the model. 142 Running the Analysis : Contact Analysis (Nonlinear Material) Running the Analysis : Contact Analysis (Nonlinear Material) File LUSAS Datafile… A LUSAS data file name of vnotch_nonlinear_contact will be automatically entered in the File name field. • Ensure that the options Solve now and Load results are selected. • Click the Save button to finish. A LUSAS Datafile will be created from the model information. The LUSAS Solver uses this datafile to perform the analysis. If the analysis is successful... The LUSAS results file will be added to Load Case section of the Treeview. In addition, 2 files will be created in the directory where the model file resides: vnotch_nonlinear_contact.out this output file contains details of model data, assigned attributes and selected statistics of the analysis. vnotch_nonlinear_contact.mys this is the LUSAS results file which is loaded automatically into the Treeview to allow results processing to take place. If the analysis fails... If errors are listed that for some reason you cannot correct, a file is provided to recreate the model information correctly, allowing a subsequent analysis to be run successfully. vnotch_nonlinear_contact_modelling.vbs complete modelling of the example. File New… carries out Start a new model file. If an existing model is open Modeller will prompt for unsaved data to be saved before opening the new file. • Enter the file name as vnotch_nonlinear_contact File Script Run Script... File LUSAS Datafile... the > To recreate the model, select the file vnotch_nonlinear_contact_modelling.vbs located in the \\Examples\Modeller directory. Rerun the analysis to generate the results 143 Elasto-Plastic Analysis of a V-Notch Viewing the Results : Contact Analysis (Nonlinear Material) If the analysis was run from within LUSAS Modeller the results will be loaded on top of the current model and the loadcase results for each load increment can be seen in Treeview. Load increment 1 is set to be active by default. the Changing the Active Results Loadcase • In the Treeview right-click on the last load increment (for load factor 2.5) and select the Set Active option. Preparing to animate the spread of yielded material As an alternative to viewing results individually for each loadcase, the change of stress and the spread of yielded material due to the increasing load increments can be animated instead. Stress contours and yield symbols will be plotted for selected load increments. • If present, delete the Mesh, Geometry and Attributes layer names from the Treeview. • With no features selected click the right-hand mouse button in a blank part of the graphics window and select the Deformed mesh option to add the deformed mesh Treeview. layer to the • On the Deformed mesh dialog click the Specify factor option and enter a Factor of 1 and click the OK button. Note. When animating nonlinear loadcases it is important that the deformed mesh is plotted using a specified factor of 1 and not using a fixed screen size value of magnitude otherwise the deformed mesh for each load increment would be drawn the same. • With no features selected click the right-hand mouse button in a blank part of the graphics window and select Contours to add the contours layer to the Treeview. The contour plot properties will be displayed. • Select Stress - Plane Stress contour results of Equivalent stresses SE • Select the Contour Range tab and set the Maximum contour value as 300 • Click the OK button. 144 Viewing the Results : Contact Analysis (Nonlinear Material) The contour plot and contour summary for load increment 25 will be displayed showing the region of yielded material has spread across the whole arm of the model. • If necessary, change the layer display order to display the deformed mesh on top of the contour plot by moving the Deformed Treeview. mesh to follow Contours in the • With no features selected click the right-hand mouse button in a blank part of the graphics window and select Values to add the values layer to the Treeview. The values layer properties dialog will be displayed. • Select Stress - Plane Stress values of component Yield • Click the OK button to display yield symbols for load increment 25 to show areas of the model that have yielded. • Select No to not change the contour layer to match. Animating the results Utilities Animation Wizard… • Select the Load history option and click the Next button. • Select vnotch_nonlinear_contact.mys from the drop-down menu. The list of available load cases for selection will appear. Note. With so many load increments there is no need to animate the whole sequence. The selected load cases can be filtered to reduce the number to be animated. • Enter a Step value of 4 to display every fourth increment and click the Filter button. The filtered load increments will displayed in the loadcase panel. 145 Elasto-Plastic Analysis of a V-Notch • Select the first load increment, hold down the Shift key and select the last load increment. button to add the selected load increments to the included panel • Click the for the animation sequence. • Click the Finish button to create the animation sequence and display the animation in a new window. Note. To see the animation at the best resolution enlarge the window to a full size view. The buttons at the bottom of the window may be used to slowdown, speed-up, pause, step through frame by frame, or stop the animation. Saving Animations Animations may be saved for replay in LUSAS at any time or saved for display in other windows animation players. • Ensure the animation window is the active window. File Save As AVI... • Enter vnotch_nonlinear_contact for the animation file name. An .avi file extension is automatically appended to the file name when it is saved. • Animations can be compressed to save disk space. A number of compression formats are available depending on what is installed on the system. Microsoft Video 1 has been found to provide reliable results. • Click OK to create the animation file. 146 Viewing the Results : Contact Analysis (Nonlinear Material) This completes the example. 147 Elasto-Plastic Analysis of a V-Notch 148 Description Modal Analysis of a Tuning Fork For software product(s): With product option(s): All. None. Description This example demonstrates a natural frequency analysis of a stainless steel tuning fork. The dimensions are those of an A tuning fork which vibrates at 440 Hz. The overall dimensions of the fork are as shown. 134.5 93.25 52.0 R=20.0 R=1.5 7.5 3.5 3.5 23.0 R=3.5 2.0 4.0 44.0 All Dimensions are in mm 48.5 Units of N, mm, t, s, C are used throughout. For natural frequency analysis consistent units must be adopted. A model for an eigenvalue analysis is created in an identical way to that required for a static analysis, using features and attributes, but a relatively coarse mesh is used since stress output is not required. No loading is applied to the structure. Eigenvalue control data is included to specify details of the analysis required. In a natural frequency analysis the following assumptions are made: There is no applied load and vibration is due to the mass and stiffness of the structure alone. 149 Modal Analysis of a Tuning Fork There is no damping. Vibration assuming sinusoidal displacements of the form a = ASin(ωt). The numerical solution produces a series of eigen pairs. The eigenvalues which indicate frequencies at which the vibration would naturally occur are output. The eigenvectors give the associated mode shape of vibration. It is important to note that the solved eigenvectors (and hence the resulting mode shape displacements) are normalised and hence may be arbitrarily scaled. Although displacement, strain and stress information may be plotted, these quantities are therefore only relative and cannot be used directly in the design process. It is common for the magnitudes of these quantities to be investigated by running subsequent modal analyses such as forced (harmonic) or spectral (seismic) response. In this case the resulting eigenvalues will be manipulated interactively during results processing using the Interactive Modal Dynamics (IMD) facility. The default method for Eigenvalue Extraction, used here, is Subspace Iteration. This method has the following characteristics: All of the degrees of freedom in the model are used in the solution. An initial estimated solution is improved via subsequent iterations. These characteristics make the method very accurate and robust. Keywords 2D, Intersecting Features, Splitting Features, Surfaces by Joining, Mirroring, Natural Frequency, Eigenvalue, Eigenvalue Control, Interactive Modal Dynamics (IMD), Mode Shapes, Animation, Frequency Response Graphs. Associated Files fork_modelling.vbs carries out the modelling of the fork. Modelling Running LUSAS Modeller For details of how to run LUSAS Modeller see the heading Running LUSAS Modeller in the Examples Manual Introduction. Note. This example is written assuming a new LUSAS Modeller session has been started. If continuing from an existing Modeller session select the menu command File>New to start a new model file. Modeller will prompt for any unsaved data and display the New Model dialog. 150 Modelling Creating a new model • Enter the file name as fork • Use the Default working folder. • Enter the title as Tuning Fork - Frequency Analysis • Set the units to N,mm,t,s,C • Select the model template Standard • Ensure the Structural user interface is selected. • Select the Vertical Y Axis option and click the OK button. Note. Save the model regularly as the example progresses. Use the Undo button to correct any mistakes made since the last save was done. Feature Geometry Geometry Line > Arc/Circle From Coords/Points … • Enter coordinates of (0, 0), (1.5, 0), and (1.5, 1.5) to define the arc at the far left end of the fork. Select the coordinate (1.5, 0) as the Centre of the arc and click OK • Drag a box to select the 2 Points shown. Select these 2 Points Use the New Line button to create the Line. • Select the other 2 Points shown. Use the New Line button to create the Line. • Select the Arc, hold down the Shift key and then select the 2 straight Lines by individually clicking on each in turn. Select these 2 Points Using the New Surface button, create a Surface from the Lines selected. • Click on a blank part of the graphics window to clear the selection. Geometry Point Coordinates... > Define Points at coordinates of (23,0) and (23,3.5) and click OK • Select pairs of Points and create new Lines between each pair. 151 Modal Analysis of a Tuning Fork • Drag a box around these Lines. Create a Surface to form the next part of the base of the fork. Geometry Point Coordinates... > Select these 4 Lines Click on a blank part of the graphics window to clear the selection and then Define Points at coordinates of (44,0) and (44,7.5) which form the ends of the radius handle of the fork. • Select pairs of Points and use the New Line button to create only the straight Lines shown. • To define the arc. Select the arc start and end Points, and the Point at the bottom right of the model. 2. Select this Point 1. Select this Point 3. Select this Point 152 Modelling Geometry Line > Arc/Circle From Coords/Points… • Specify that coordinate (44,0) is a Direction Point. • Ensure that Minor arc is selected • Enter an arc radius of 20 • Click OK to draw the arc. The Lines which mark the extent of the support conditions on the handle (that is the area over which the fork is assumed to be held) will now be defined. This will be done by copying existing Lines. • Select the first Line shown. 2. Select this Line 1. Select this Line Copy the Line once through a distance of 2 in the X direction and click OK • Select the second Line shown Copy the Line once through a distance of -4 in the X direction and click OK 153 Modal Analysis of a Tuning Fork Points are now created at the intersections of the arc with the 2 new copied Lines. 1. Select these 3 Lines 2. Select this Line and these 2 Points • Select the 3 upper Lines shown using the Shift key to add to the initial selection. Geometry Point > By Intersection.. • Create Exact intersections only and ensure the Split intersecting lines and Delete geometry on splitting options are selected. Click the OK button to create the new Points at the Line intersections and also split the selected Lines. In order to create 3 separate Surfaces the Line along the axis of symmetry has to be split into 3 new Lines. • Select the Line and 2 Points shown in the previous diagram. Geometry Line By Splitting At a point … > > • Ensure that Delete features on splitting is selected and click OK to create 3 new Lines. Three Surfaces are now defined using the Lines previously created. • Select the 4 Lines (remembering to hold the Shift key down after the first line is selected to add to the selection) to form the boundary of the Surface shown. Select these 4 Lines to create a Surface Create a Surface here also Create a Surface here also Geometry Surface Lines... > Use the New Surface button to create a Surface. • Repeat, selecting each set of 4 Lines to define the remaining 2 Surfaces 154 Modelling Lines and Points that are left over from the previous operations can be deleted to tidy-up the model. • Drag a box around the features shown, ensuring that no Surfaces are selected. Select these features only Edit Delete To delete the unwanted Lines. • Select Yes to delete Lines. • Select Yes to delete Points. Note. Only those Point and Line features that are not used to define any Surfaces will be deleted. • Click on a blank part of the graphics window to clear the selection. Geometry Point Coordinates... > Enter coordinates of (48.5,0) and (52,7.5) and click OK to define the points. A horizontal Line will now be created. • Select the two Points and create the horizontal straight Line as shown above. 155 Modal Analysis of a Tuning Fork Now define the arc at the start of the arm section of the fork. Select this Point to create arc (52,0,0) • Select the single Point. Geometry Line > Arc/Circle > By Sweeping Points… Select the Rotate option to sweep the point through an angle of -90 degrees about the Z-axis around an origin Point of (52, 0, 0) • Click OK to sweep the Point and create an Arc. To avoid the creation of a 5-sided Surface at the start of the arm section the arc will be split into two. • Select the newly created arc. Geometry Line By Splitting In equal divisions… > > • Enter 2 for the number of divisions. Ensure Delete original lines after splitting is selected and click OK to replace the arc with two new arcs. To complete the junction section of the fork two new Surfaces will be defined. Select this Line Select this arc Zoom in to the working area. Revert to standard cursor mode and select one of the Arcs. Hold down the Shift key and select the Line on the opposite side as shown above. Geometry Surface By Joining… > Create the first Surface. • Repeat the previous procedure to create the second Surface as shown below. 156 Modelling The remainder of the fork will be created by sweeping the vertical Line at the righthand end of the model through a distance in the X direction. Resize the model so all features are in view. • Select the vertical Line shown. 1. Select this vertical Line to create Surface Geometry Surface > By Sweeping… 2. Select this vertical Line to create Surface Enter a distance of 41.25 in the X direction. • Click OK to create the Surface. • Select the new Line at the right-hand end of the model. Geometry Surface > By Sweeping… Use the Sweep Feature button to sweep the Line through a distance of 41.25 in the X direction to create the Surface. The geometry of the half-model of the tuning fork is now complete. Attribute data such as mesh, loading and supports will now be added to the half-model before copying and mirroring to create a full model for analysis. Meshing A frequency analysis can use a relatively coarse mesh, since stress output is not required from the analysis. With this in mind, a series of Line meshes will be used to control the density of the Surface mesh. Line meshes As the majority of the Lines require only 2 divisions the default number of mesh divisions will be reset. 157 Modal Analysis of a Tuning Fork • Select the Meshing tab, set the default number of divisions to 2 and click OK to return to the graphics window. Any Lines to which a line mesh dataset is not assigned will adopt this as a default. File Model Properties… Selected Lines will be assigned a number of Line divisions. LUSAS provides a limited number of Line Mesh datasets by default. These can be found in the Treeview. A Line mesh dataset with 12 divisions is not defined by default so one must be created. Attributes Mesh Line… > • With the Element description set as None, define a Line mesh dataset containing 12 divisions named Divisions=12 • Click OK to add the dataset name to the Divisions=1 Divisions=3 Divisions=4 Treeview. Divisions=12 Divisions=12 Divisions=4 Divisions=3 Divisions=1 • With the relevant sets of Lines selected, drag and drop the appropriate Line mesh datasets from the Treeview onto the selected features. Use the Zoom in button as necessary. Surface mesh Attributes Mesh Surface… > • Define a Surface mesh using Plane Stress, Quadrilateral, Quadratic elements. Name the dataset Plane Stress and click OK • Using the Ctrl and A keys together Select the half model of the fork. • Drag and drop the Surface mesh dataset Plane Stress from the the selected features. 158 Treeview onto Modelling Note. Since all of the Surfaces are 4 (or 3) sided, a regular mesh pattern is created. At any time the mesh (and other layers) displayed in the graphics window may be hidden or redisplayed. With no features selected click the right-hand mouse button in a blank part of the graphics window and select Mesh. If a mesh was previously displayed it will be hidden. If previously hidden it will be displayed. This facility can be used to simplify the display when it is required. • Remove the Mesh from the display as described in the previous note. Geometric Properties Attributes Geometric Surface… > • Specify a thickness of 4 and leave the eccentricity blank. • Enter the dataset name as Thickness and click OK. • With the whole model selected (Using the Ctrl and A keys together) drag and drop the geometry dataset Thickness from the Treeview onto the selected features. Geometric assignments are visualised by default. Use the fleshing on/off button to turn off the geometry visualisation. Material Properties Attributes Material > Material Library… • Select Stainless Steel of grade Ungraded and click OK • With the whole model selected, drag and drop the material dataset Stainless Steel (N,mm,t,s,C) from the Treeview onto the selected features. • Ensure the Assign to surfaces option is selected and click OK Support Conditions LUSAS provides the more common types of support by default. These can be seen in the Treeview. To model the holding of the tuning fork the support dataset Fixed in XY will be used. 159 Modal Analysis of a Tuning Fork Note. 2D plane stress elements only have X and Y degrees of freedom therefore a restraint in the Z direction is not necessary. • With the arc shown in the diagram selected, drag and drop the support dataset Fixed Treeview in XY from the onto the selected Line. Select this Line • Ensure the Assign to lines and All loadcases options are selected and click OK • If supports are not visualised when expected they can be visualised for each support condition by right-clicking on the support name in the supports section of the Treeview and selecting Visualise Assignments. Note. In practice this support would not be a rigid support since it is hand held but this should not significantly affect the frequencies obtained. Loading No loading is required for a natural frequency analysis. Note. The fork is symmetrical about its centre-line, therefore only half of the structure has so far been created. For static structural analysis it would be common to apply a symmetry support condition to the centreline, so that only half of the structure need be analysed. However, in a frequency analysis the use of symmetry in this way is less common since this will force the analysis to only solve for the symmetric modes of vibration ignoring any anti-symmetric modes. Generally, both symmetric and anti-symmetric vibration modes are of significance, therefore the model will be mirrored to form the complete model. Select these 2 Points to define mirror plane • Select the 2 Points on the centreline of the tuning fork as shown. 160 Modelling Edit Selection Memory > Set Geometry Surface Copy… The Points are stored in memory. • Select the whole model using the Ctrl and A keys together. Select Mirror - points 5 7 from the drop-down list and click the Use button on the dialog to use the Mirror Points stored in memory. • Click OK to create the full model. Edit Selection Memory > Clear To remove the Points from the selection memory. Note. The model is 2 Dimensional, therefore only 2 Points are required to define the mirror plane (the Z direction is assumed as the screen Z plane). In addition, the selection of Points as far away from each other as possible will ensure a good specification of the required mirror plane. The model is now complete. All attributes assigned to the original half-model features, including the support and mesh assignments, will have been identically reproduced on the duplicated features. Eigenvalue Analysis Control The eigenvalue analysis control parameters are applied as properties of the load case. • In the Treeview right-click on Loadcase 1 and select Eigenvalue from the Controls menu option. The Eigenvalue dialog will appear. 161 Modal Analysis of a Tuning Fork The following parameters need to be specified to perform a frequency analysis with a specified number of the minimum eigenvalues. • Set the Number of eigenvalues required to 10 • Set the Shift to be applied to 0 • Leave the type of eigensolver as Default Note. Eigenvalue normalisation is set to Mass by default. This is essential if the eigenvectors are to be used for subsequent IMD analysis in results processing as they are in this case. • Click the OK button to finish. Saving the model File Save Save the model file. Running the Analysis With the model loaded: File LUSAS Datafile... A LUSAS data file name of fork will be automatically entered in the File name field. • Ensure that the options Solve now and Load results are selected. • Click the Save button to finish. A LUSAS Datafile will be created from the model information. The LUSAS Solver uses this datafile to perform the analysis. If the analysis is successful... LUSAS eigenvalue results will be added to Treeview. In addition, 2 files will be created in the directory where the model file resides: fork.out this output file contains details of model data, assigned attributes and selected statistics of the analysis. fork.mys this is the LUSAS results file which is loaded automatically into the Treeview to allow results processing to take place. 162 Viewing the Results If the analysis fails... If the analysis fails, information relating to the nature of the error encountered can be written to an output file in addition to the text output window. Any errors listed in the text output window should be corrected in LUSAS Modeller before saving the model and re-running the analysis. Rebuilding a Model If it proves impossible for you to correct the errors reported a file is provided to enable you to re-create the model from scratch and run an analysis successfully. fork_modelling.vbs carries out the modelling of the example. File New… Start a new model file. If an existing model is open Modeller will prompt for unsaved data to be saved before opening the new file. • Enter the file name as fork File Script Run Script... File LUSAS Datafile... > To recreate the model, select the file fork_modelling.vbs located in the \\Examples\Modeller directory. Rerun the analysis to generate the results Viewing the Results This section outlines some typical results processing operations for a natural frequency and Interactive Modal Dynamics (IMD) analysis. The following interactive results processing operations are performed: Mode Shape Plots Displaying mode shapes from the natural frequency analysis. Mode Animation Sequence Animation of selected mode shapes. Printing Eigenvalue Results Printing results to a text window. Modal Dynamics (IMD) Graphing of Displacement vs. Frequency for a selected node (all frequencies) using a linear scale. 163 Modal Analysis of a Tuning Fork Selecting a Results Loadcase If the analysis was run from within LUSAS Modeller the results will be loaded on top of the current model and the load case results for eigenvalue 1 are set to be active by default. Plotting Mode Shapes If present, delete the Geometry, Attributes and Mesh layers from the Treeview. • With no features selected click the right-hand mouse button in a blank part of the Graphics window and select Deformed mesh to add the deformed mesh layer to the Treeview. • Click the OK button and the deformed mesh plot for Eigenvalue 1 will be displayed. Note. The mode shape may be inverted. This is because the sense is arbitrary since during vibration the deformed shape will appear in both directions. To view other mode shapes, in the Treeview right-click on the Eigenvalue required and select the Set Active option. Creating Animations of Mode Shapes This section will create an animation of the third mode shape. • In the Treeview right-click on Eigenvalue 3 and select the Set Active option. • The deformed shape for Eigenvalue 3 will be displayed. Utilities Animation Wizard... • Select the Active loadcase button and select the Next button. • Use a Sine deformation with 8 frames. Set the range to –1 to 1. Set the deformation magnitude of 6 mm. • Click Finish and LUSAS will create the animation sequence and display the animation in a new window. 164 Viewing the Results • To see the animation at the best resolution enlarge the window to full size. The buttons at the bottom of the window may be used to slow-down, speed-up, pause, step through frame by frame, or stop the animation. Saving Animations Animations may be saved for replay in other windows animation players. • Ensure the animation window is the active window. File Save As AVI... • Enter fork_mode3 for the animation file name. An .avi file extension is automatically appended to the file name when the file is saved. • Animations can be compressed to save disk space. A number of compression formats are available depending on what is installed on the system. Microsoft Video 1 has been found to provide reliable results. Click OK. Close the animation window without saving changes. 165 Modal Analysis of a Tuning Fork Printing Eigenvalue Results Eigenvalue results for the model can be displayed in the Text Output window. Utilities Print Results Wizard… • Select Entity None of results Type Eigenvalues and click the Finish button to print the eigenvalues to the text output window. Your values should be similar to these: Results File Eigenvalues MODE = C:\Lusas140\Projects\fork.mys ID=0 EIGENVALUE FREQUENCY ERROR NORM 1 0.725647E+07 428.729 0.137567E-08 2 0.740305E+07 433.037 0.136178E-08 3 0.272988E+09 2629.61 0.461326E-10 4 0.283643E+09 2680.44 0.430260E-10 5 0.200119E+10 7119.74 0.392818E-10 6 0.214224E+10 7366.38 0.127963E-10 7 0.375775E+10 9756.28 0.252194E-10 8 0.572457E+10 12041.8 0.139476E-10 9 0.668763E+10 13015.4 0.258395E-09 10 0.810989E+10 14332.7 0.956746E-07 Note. The error norms may vary as they are dependent on the Eigensolver used for the solution. Close the text window. Interactive Modal Dynamics The vertical displacement response of a selected node for a unit vertical force is to be plotted against the sampling frequency over the entire solved frequency range (0-15000 Hz) on a linear scale. • Select the node at the end of the arm shown. Select this Node 166 Viewing the Results Using the Graph Wizard The graph wizard provides a step-by-step means of selecting results to be plotted on the X and Y axes of a graph. The X axis data is always defined first. Utilities Graph Wizard... • Select the Modal Expansion option and click the Next button. • The Frequency response for All modes is to be calculated for the X axis data. Ensure the Damping Type is set to None • On the Modal Excitation section of the dialog ensure that Point excitation is selected and click the adjacent Set button. • Select the Node number previously selected from the drop-down list. Select component DY and click the OK button to return to the main dialog. • Click the Next button. The excitation loading has been defined. The response has now to be defined. • On the Modal Frequency Domain dialog select Displacement results of component DY. Enter Sampling frequency values of Start as 0, End as 15000 and Step as 100 • Click the Next button. The response has now been defined. Frequency (X) and Amplitude (Y) axis datasets are now generated to graph the displacement frequency response at the selected node. Additional information for the graph can now be added. • Leave all graph title information blank. • De-select the Show symbols button. • Click the Finish button to end. Note. If no graph or axis titles are entered default names will be used. The graph attributes may be edited by right clicking on the graph and selecting Edit Graph Properties 167 Modal Analysis of a Tuning Fork LUSAS will create the graph in a new window and display the values used in an adjacent table. To see the graph at the best resolution enlarge the window to a full size view. Note. By using a large frequency range with a 100Hz interval the peak amplitude at the frequency of 438Hz can be missed when plotting graphs of this nature. It is better to use a smaller frequency range in order to isolate the peak results. To produce a more accurate graph and with the same node selected: • Close the current graph window. Utilities Graph Wizard... • With the Modal Expansion option selected click the Next button. • With all options that were set previously selected click the Next button. • Select Displacement results of component DY. Enter sampling frequency values of Start as 0, End as 800 and Step as 1 • Click the Next button. • Leave all graph title information blank. • Ensure the Show symbols option is not selected • Click the Finish button to end. 168 Viewing the Results LUSAS will create the graph in a new window and display the values used in an adjacent table. To see the graph at the best resolution enlarge the window to a full size view. This displays a better representation of the displacement/ frequency response in the vicinity of the first mode shape. Plotting Dynamic Response for a Particular Frequency In some analyses, dynamic responses are required at a specified frequency. In these cases, an Interactive Modal Dynamics (IMD) load case is defined to allow the frequency and type of excitation to be specified. In this example, deformed shapes and peak displacements are to be plotted for excitation frequencies of 750Hz and 1500Hz. Close all graph windows to leave the model window active. 169 Modal Analysis of a Tuning Fork Utilities IMD Loadcase On the IMD Loadcase properties dialog: • Select Point excitation and click the adjacent Set button. • Select the Node previously number selected from the dropdown list. Select component DY and click the OK button to return to the IMD Loadcase main dialog. • Select Frequency results and click the adjacent Set button. • Enter a Frequency of 750 • Click the OK button to return to the main dialog. • Ensure the name is set to be IMD 1 • Click the OK button to finish defining the IMD loadcase. Selecting the IMD Results Loadcase • In the Treeview right-click on IMD 1 and select the Set Active option. The deformed mesh plot is updated to show the deformed mesh at the specified frequency. Marking Peak Values • With no features selected click the right-hand mouse button in a blank part of the Graphics window and select the Values option to add the Values layer to the Treeview. 170 Viewing the Results • The values properties will be displayed. • Select Displacement results of displacement in the Y direction DY. Select the Values Display tab and select the top 0% of Maxima values. • Click the OK button to display the top value of displacement. Changing the results frequency • In the Treeview double-click the IMD 1 dataset name. • Click the Set button adjacent to the Frequency option. • Change the frequency to 1500 and click the OK button to return to the main dialog. • Click the OK button to finish defining the IMD loadcase. The deformed mesh plot will be updated to show the revised mode shape and corresponding values for the specified frequency. Note. Since the eigenvalue is independent of sign the deformed shape may appear inverted from that shown. This completes the example. 171 Modal Analysis of a Tuning Fork 172 Description Modal Response of a Sensor Casing For software product(s): With product option(s): All Plus Description An aerospace sensor casing is to be assessed for dynamic stresses induced by vibration of the airframe to which it is attached. The sensor casing is manufactured from steel plate with a uniform thickness of 0.8 mm. 6.0 5.0 70.0 70.0 14.14 The surfaces at the top of the sleeve Bottom Sleeve 36.0 are rigidly held. The loading is Plate All Dimensions in mm characterised by a random vibration at the supports of the airframe and is defined as an acceleration Power Spectral Density (PSD) specified by the airframe manufacturer. The Interactive Modal Dynamics (IMD) facility is used to evaluate the response of the casing to this loading. A quarter model is initially defined with the sleeve modelled as if it were in the centre of the casing, and subsequently copied to create the full model. The sleeve is then repositioned to the location shown to show the associativity of features. Units of N, m, kg, s, C are used for the analysis. 173 Modal Response of a Sensor Casing Objectives The following results plots are to be obtained: Deformed Shape A display of the deformed mesh for the first mode shape. Frequency Response Function FRF of a node using support motion excitation. Power Spectral Density PSD stress response at a node using a PSD excitation function. Keywords Linear, Eigenvalue, Scale Factor Transformation, Interactive Modal Dynamics (IMD), Default Attribute Assignment, Deformed Shape, Frequency Response Function (FRF), Power Spectral Density (PSD), Stress Contours. Associated Files casing_modelling.vbs carries out the modelling of the example. Modelling Running LUSAS Modeller For details of how to run LUSAS Modeller see the heading Running LUSAS Modeller in the Examples Manual Introduction. Note. This example is written assuming a new LUSAS Modeller session has been started. If continuing from an existing Modeller session select the menu command File>New to start a new model file. Modeller will prompt for any unsaved data and display the New Model dialog. Creating a new model • Enter the file name as casing • Use the Default working folder. • Enter the title as Modal Response of Sensor Casing • Set the units as N,m,kg,s,C 174 Modelling • Select the model template Standard • Ensure the Structural user interface is selected • Select the Vertical Y axis. • Click the OK button. Note. Save the model regularly as the example progresses. Use the Undo button to correct any mistakes made since the last save was done. Default assignments The material properties, plate thickness and mesh element type are uniform over the whole sensor casing. By using default attribute assignments, attribute datasets are automatically added to new features when they are created. Automatic Mesh Assignment Attributes Mesh Surface... > • Define a Surface mesh using Thin shell, Quadrilateral elements with Linear interpolation. • Enter Thin shell for the mesh dataset name. • Click the OK button to add the mesh dataset to the Treeview. • To set this mesh dataset as the default surface mesh assignment click the righthand mouse button on the Thin shell dataset name in the Treeview and select the Set Default option. The icon will change to indicating that Thin shell will automatically be assigned to all new Surfaces. Automatic Geometry Assignment Attributes Geometric Surface... > • Enter a Surface element thickness of 0.0008 • The eccentricity can be left blank or set to zero as it is not required. • Enter the dataset name as Thickness of 0.0008 and click OK to add the dataset to the Treeview. • To set this geometry dataset as the default geometry assignment click the right-hand mouse button on the Thickness of 0.0008 dataset name in the Treeview and select the Set Default option. 175 Modal Response of a Sensor Casing Automatic Material Assignment Attributes Material > Material Library... • The sensor is made from steel so select Mild Steel from the drop down list. • Click OK to add the material to the Treeview. • Set this material as the default material assignment by clicking the right-hand mouse button on the Mild Steel Ungraded (N,m,kg,s,C) material dataset in the Treeview and selecting the Set Default option. Feature Geometry In a natural frequency analysis, consistent units such (N, m, kg, sec) must be used. It is however more convenient to define the geometry in millimetres and scale the model when the geometry input is complete. Defining the sleeve of the sensor Note. The sleeve is defined initially as if it were positioned centrally on the casing. Later in the example it will be moved to its actual position to show the associativity of features. Geometry Line Coordinates... > Define a Line on the sleeve from (0,0) to (-5,-5) and click the OK button. • Select the Line just drawn. Geometry Surface By Sweeping... > Sweep the line into a surface by choosing the Rotate option and entering an angle of 90 degrees to rotate the line about the Z-axis about an origin of 0,0,0 • Click the OK button to complete the Sweep operation. Select the fleshing on/off button to turn-off geometric property visualisation. The number of elements modelling the end of the sleeve will be reduced. 176 Modelling • Select the two radial Lines and adjust the mesh by assigning Line mesh Division=1 from the Treeview. Select these two lines Defining the mesh for the sleeve The arc will now be swept to create a Surface. • Select the arc Geometry Surface By Sweeping... > Sweep the arc into a surface by selecting the Translate option and enter a translation of -5 in the Z direction. Click the OK button to create the surface. Use the Isometric view button to view the Surface created. The sides of the sensor will now be defined. Note. To simplify the modelling the sleeve will be defined at the centre of the plate and moved when the full model has been generated. Geometry Line Coordinates... > Enter coordinates of (-35, -35, -5) and (35, -35, -5) to define a Line representing the bottom edge of the housing. Click OK to generate the Line. A new Surface can be created by joining this new Line to the previously defined arc to form a quarter of the housing plate. 177 Modal Response of a Sensor Casing • Select the arc shown right and add the Line at the bottom edge of the sensor to the selection by hold down the Shift key. Geometry Surface By Joining... 1. Select this arc A Surface will be created. > The Line at the bottom edge of the sensor casing is now to be swept to create the bottom Surface of the casing. • Select the bottom edge Line of the housing. Geometry Surface > By Sweeping… Choose the Translate option and define a translation of -30 in the Z direction. Click the OK button to create the new Surface. Sweep this line through -6 units in the Z direction To define the portion of casing beyond the bottom plate, select the Line shown. Geometry Surface > By Sweeping… Define a translation of -6 in the Z direction and click OK to sweep a new Surface. • Now adjust the mesh on the new surface by selecting the 2 Lines of the casing indicated in the diagram and drag and drop the Line mesh Divisions=1 from the Treeview onto the selected features. Select these 2 lines and assign Line Mesh Divisions=1 This completes the definition of the features of the quarter model. 178 2. Select this line Modelling Supports Note. Supports are to be assigned to the quarter model before copying is done to save time assigning the support dataset to the equivalent copied Surfaces. • Select the Surface at the end of the sleeve. If necessary, zoom in and cycle though the displayed features by clicking the left-hand mouse button until the Surface required is highlighted. • Drag and drop the support dataset Pinned from the Treeview onto the selected surface and click OK The full housing model can now be created from the quarter model • Using the Ctrl and A keys together, select the whole model. Geometry Surface Copy… > Use the copy button to Rotate the selected features through 90 degrees about the Z-axis and create 3 copies of the original selection. • Click OK and Modeller will create and display the extra features. • To generate the bottom plate select the 4 Lines shown. Geometry Surface Lines... > The Surface defining the bottom plate will be created. Finally the sleeve must be moved off centre. Rotate the model to view along the Z axis by clicking in the status bar at the bottom of the Modeller window. • For clarity delete the Mesh and Attributes layers from the Treeview. 179 Select these 4 lines Modal Response of a Sensor Casing • Box select the features which make up the sleeve. Select the Sleeve Geometry Point Move... > Move the sleeve to the required position by entering a translation of -7.07 in the X direction and -7.07 in the Y direction and click OK Finally the geometry must be scaled so the units are metres. • Use the Control and A keys together to select the full model. Geometry Point Move... > Select the Scale option and enter a scale factor of 0.001 about an origin of 0,0,0. • Click OK to scale the geometry from millimetres to metres. Eigenvalue Analysis Control To carry out results processing using the Interactive Modal Dynamics facility, an eigenvalue analysis must be performed. The results from the eigenvalue analysis normalised to global mass will be used to perform the Frequency Response Function calculations. The eigenvalue analysis control properties are applied as a function of the load case. 180 Running the Analysis • In the Treeview right-click on Loadcase 1 and select Eigenvalue from the Controls menu option. The Eigenvalue dialog will appear. The following parameters need to be specified to perform a frequency analysis with the minimum number of eigenvalues. • Set the Number of eigenvalues required as 8 • Set the Shift to be applied as 0 • Leave the type of eigensolver as Default Note. Eigenvalue normalisation is set to Mass by default. This is essential if the eigenvectors are to be used for subsequent IMD analysis in results processing as in this case. • Click the OK button to finish. Saving the model The model is now complete. File Save Save the model file. Running the Analysis With the model loaded: 181 Modal Response of a Sensor Casing File LUSAS Datafile... A LUSAS data file name of casing will be automatically entered in the File name field. • Ensure that the options Solve now and Load results are selected. • Click the Save button to finish. A LUSAS Datafile will be created from the model information. The LUSAS Solver uses this datafile to perform the analysis. If the analysis is successful... The LUSAS results will be added to the Treeview. In addition, 2 files will be created in the directory where the model file resides: casing.out this output file contains details of model data, assigned attributes and selected statistics of the analysis. casing.mys this is the LUSAS results file which is loaded automatically into the Treeview to allow results processing to take place. If the analysis fails... If the analysis fails, information relating to the nature of the error encountered can be written to an output file in addition to the text output window. Any errors listed in the text output window should be corrected in LUSAS Modeller before saving the model and re-running the analysis. Rebuilding a Model If it proves impossible for you to correct the errors reported a file is provided to enable you to re-create the model from scratch and run an analysis successfully. casing_modelling.vbs carries out the modelling of the example. File New… Start a new model file. If an existing model is open Modeller will prompt for unsaved data to be saved before opening the new file. • Enter the file name as casing and click OK File Script Run Script... File LUSAS Datafile... > To recreate the model, select the file casing_modelling.vbs located in the \\Examples\Modeller directory. Rerun the analysis to generate the results 182 Viewing the Results Viewing the Results This section outlines some typical results processing operations for a natural frequency and Interactive Modal Dynamics (IMD) analysis. The following interactive results processing operations are performed: Mode Shape Plots Displaying mode shapes from the natural frequency analysis. Frequency Response Function (IMD) Graphing of Acceleration due to support motion vs. Frequency for a selected node (all frequencies) using a linear scale. Power Spectral Density Response (IMD) Displaying the PSD stress response for a node on the top plate due to a PSD acceleration input at the supports. Selecting a Results Loadcase If the analysis was run from within Modeller the results will be loaded on top of the current model and the loadcase results for each eigenvalue can be seen in the Treeview. Displaying the 1st Mode Shape • Delete the all layers from the Treeview. • Ensure Eigenvalue 1 is active in the Treeview. • With no features selected click the right-hand mouse button in a blank part of the graphics window and select Deformed mesh to add the deformed mesh layer to Treeview. the • Change the specified magnitude to 20 and click the OK button to display the deformed mesh for eigen mode 1. 183 Modal Response of a Sensor Casing Use the Dynamic Rotation button to rotate the model to a similar view to that shown. Return to normal cursor mode. Note. For more complex mode shapes it may be beneficial to animate the mode shape so it can be seen in more detail. Note. In some cases the mode shape may appear inverted. This is because the Eigenmode represents the shape of the vibrating body and the displacements may be multiplied by -1. Stresses as Filled Contours • Delete the Deformed mesh layer from the Treeview • With no features selected click the right-hand mouse button in a blank part of the graphics window and select Mesh to add the mesh layer to the Treeview and click OK to accept the default properties. • Transform the view to visualise model from the X direction in clicking on the status bar at the bottom of Modeller window. the by the the • Select an area enclosing the top plate of the housing as shown. Select elements on top plate by boxing region shown. Create a new group consisting of the elements forming the top plate. • Enter Top Plate as the group name and click OK. Rotate the model to view along the Z axis by clicking in the status bar at the bottom of the Modeller window. • Make the top plate the only visible part of the model by clicking with the righthand mouse button on Top Plate in the Treeview and selecting Set as Only Visible 184 Viewing the Results • Ensure the results for Eigenvalue 1 are set active in the Treeview. • With no features selected right-click on a blank part of the screen and select Contours • Select the Stress (top) – Thin Shell entity and maximum absolute stress component Sabs • Click the OK button to display contours of maximum absolute stress. • To display the mesh on top of the contours select Mesh in the Treeview and drag and drop it on top of the Contours layer name. Highest stressed node. The node where the maximum absolute stress occurs is noted at the bottom of the contour key. • Make a note of this node number as it will be used later in the example. Note. The contours are relative stress contours which have no quantitative meaning. Interactive Modal Dynamics Note. A FRF (frequency response function) is a transfer function in the frequency domain. In general terms, the transfer function indicates how much of the input excitation is transferred to the selected output point. Compute the modal acceleration response in the Z direction at the node in the centre of the bottom surface due to a harmonically varying acceleration applied to the structural supports. • Delete the Contours layer from the Treeview. • Redisplay the full model by selecting the casing.mdl in the right-hand mouse button and selecting Set as Only Visible. 185 Treeview with the Modal Response of a Sensor Casing Rotate the model as shown Return to normal cursor mode. • Select the node at the centre of the bottom plate. Select this node at centre of back plate Utilities Graph Wizard… • Select the Modal Expansion option and click the Next button. • On the Modal Dynamics Graph dialog choose the Frequency entity. • Under the damping section choose Specified values from the drop down list. 186 Viewing the Results • Select the Set damping button and set the viscous damping to 0 and the structural damping to 2.8 • Click the OK button to return to the Modal Dynamic Graph dialog. Note. If damping values are specified for the first mode only, the other modes will take the same values. • From the Modal Excitation drop down list select Support Motion • Click on the Set button and on the Support Motion dialog specify Acceleration in the Z direction. • Click the OK button to return to the Model Dynamics Graph dialog and click Next • On the Modal Frequency Domain dialog select the Displacement entity in the DZ direction. • Set the calculated entity as Acceleration of Type Amplitude. The selected node number at the centre of the back plate will be displayed in the drop down node list. • Set the sampling frequencies start, end and step entries to 50, 187 Modal Response of a Sensor Casing 3000 and 5 respectively. • Click Next • On the Display Graph dialog ensure that the Show symbols option is not selected. • In the Y Scale section select the Use logarithmic scale option. • Click on the Finish button and a graph of log acceleration against frequency will be plotted. • To specify axis labels and title right click on the graph and select Edit graph properties • On the General tab set the graph title to FRF in Z Direction at Centre of Back Plate (2.8% Structural Damping) • Click on the X Axis Style tab and set the axis name to Frequency (Hz) • Click on the Y Axis Style tab and axis name to Log Acceleration (m/s^2) • Click OK to update the graph display. Delete the graph window 188 Viewing the Results Power Spectral Density definition A PSD force input defines the frequency content of a random loading, such as turbulent pressure acting on an aircraft component. A PSD analysis is, therefore, useful when broadband random dynamic forces excite structural vibrations. Graph of PSD Stress Response • Click the left-hand mouse button in a blank part of the graphics window to clear the current selection. • Click the right-hand mouse button in a blank part of the graphics window and select the Advanced Selection option. • With the Type and name option selected, choose Node from the drop down list and enter the node number at which the maximum principal stress occurs (as noted down at an earlier stage in this example). • Click OK to add the node to the selection. Utilities Graph Wizard… • To compute a PSD stress response select the Modal expansion option and click Next • On the Modal Dynamics Graph dialog choose the Frequency entity. • Under the damping section choose Specified values from the drop down list. Select the Set damping button and set the viscous damping to 0 and the structural damping to 2.8 and click OK • From the Excitation drop down list select Support Motion • Click on the Set button and under support motion specify Acceleration in the Z direction and click the OK button to return to the Model Dynamics Graph dialog. • Click Next to move to the next dialog. 189 Modal Response of a Sensor Casing • On the Modal Frequency Domain dialog select entity Stress (top) – Thin Shell with component S1 • Set the start, end and step sampling frequencies to 50, 3000 and 5 respectively. Note. The sampling frequency range must lie within the frequency range of the PSD dataset defined earlier. • Select PSD Response from the Type drop down list and click the PSD set button. • On the RMS response for Power Spectral density dialog ensure the Linear/Linear scale option is selected and define a frequency PSD dataset using the frequency and amplitude values shown in the table on the right (Use the Tab key to create a new line in the table). • Label the dataset Frequency PSD and click OK • The selected node number will be displayed in the drop down node list. • Click the Next button. Linear Frequency Linear Amplitude 15 8 100 14 125 30 500 31 600 61 900 108 1000 79 3000 47 • On the Display Graph dialog deselect the Show grid option. Deselect the Show symbols option and select the Use Logarithmic scale option for the Y Scale. • Click the Finish button to plot a graph of log PSD against frequency. The RMS value of the input PSD and response PSD are written to the message window when the graph is plotted. 190 Viewing the Results • To specify axis labels and title right-click on the graph and select Edit graph properties • On the General tab set the graph title to Top Surface Maximum Principal Stress (2.8% Structural Damping) • Click on the X Axis Style tab and set the axis name to Frequency (Hz) • Click on the Y Axis Style tab and axis name to Log PSD • Click OK to update the graph. PSD Input The PSD input data used in the acceleration of the supports can be plotted on the same graph by following the above procedure until the Modal Frequency Domain dialog is reached. • With the node at which maximum principal stress occurs still selected, follow the steps in creating the PSD Response graph starting with the Utilities > Graph 191 Modal Response of a Sensor Casing Wizard menu option but, when the Model Frequency Domain dialog is displayed, instead of selecting PSD Response select PSD Input in the Type drop down list. • When the Display Graph dialog is reached, select the option to Add to existing graph and ensure that the Show symbols is not selected • Click Finish to update the graph. This completes the example. 192 Description Thermal Analysis of a Pipe For software product(s): With product option(s): LUSAS Analyst. Thermal Description This example provides an introduction to performing a thermal analysis with LUSAS. A continuous steel pipe is exposed to an atmospheric temperature of 25oC. Oil at 150oC 0.1m 0.05m is to be pumped through the pipe. The pipe has -1 -1 o -1 a thermal conductivity of 60 J s m C , a specific heat capacity of 482 J kg-1 oC-1 and a density of 7800 kg/m3. Two analyses will be carried out. A steady state analysis is required to determine the maximum temperature of the outer surface of the pipe and a transient thermal analysis is then performed to find out the time it will take the surface to reach this temperature once pumping begins. The units of the analysis are N, m, kg, s, C throughout. Note. There are three transport mechanisms for heat energy; conduction, convection and radiation. The first of these is defined as a material parameter, the others are defined within the load attributes as environmental variable and environmental temperatures. In this example, the effects of radiation are ignored. 193 Thermal Analysis of a Pipe Objectives The objectives of the analysis are: To determine the maximum temperature the outer surface of the pipe reaches during continual pumping. To determine how long it will take for the maximum temperature to be reached once pumping of the oil begins. Keywords Thermal, Steady State, Transient, Environmental Temperature, Prescribed Temperature. Associated Files pipe_modelling.vbs carries out the modelling of the example. Modelling Running LUSAS Modeller For details of how to run LUSAS Modeller see the heading Running LUSAS Modeller in the Examples Manual Introduction. Creating a new model File New… Start a new model file. If an existing model is open Modeller will prompt for unsaved data to be saved before opening the new file. • Enter the file name as pipe • Use the Default working folder. • Enter the title as Steady State Thermal Analysis of Pipe • Select the units as N,m,kg,s,C • Change the startup template to None • Change the user interface to Thermal • Select the Vertical Y Axis option and click the OK button. 194 Modelling Note. Save the model regularly as the example progresses. Use the Undo button to correct any mistakes made since the last save was done. Feature Geometry The pipe geometry will be generated by defining a vertical line that will be swept into a quarter segment. This segment will then be copied to generate the full model. Geometry Line Coordinates... > Enter coordinates of (0, 0.1) and (0, 0.15) to define a vertical line and click the OK button. • Select the line Geometry Surface By Sweeping... > On the Sweep dialog, choose the Rotate option and enter a rotation angle of 90 about the Z-axis. • Leave the other options and click the OK button. • Select the Surface Geometry Surface Copy... > In the Copy dialog, select the Rotate option. • Enter an Angle of 90 about the Z-axis • Enter the number of copies as 3 • Click OK to create the full pipe cross section. Meshing Plane field elements are to be used for this analysis. These elements are used to model the cross section of ‘infinite’ components since they only model heat flow in the XY plane. 195 Thermal Analysis of a Pipe Attributes Mesh Surface.. > • Select Plane field, Quadrilateral shaped, Linear elements. • Enter the attribute name as 2D Thermal Mesh and click the OK button. • Use Ctrl + A to select all the features. • Drag and drop the mesh attribute 2D Thermal Mesh from the Treeview onto the selection to assign the mesh to the selected surfaces. Geometric Properties Geometric properties are used to define the thickness of the pipe. Since the pipe is of infinite length a unit length is modelled. Attributes Geometric Surface... > • Enter a thickness of 1 and leave the eccentricity blank. • Enter the attribute name as Thickness and click the OK button. 196 Modelling • Select all the surfaces and assign the attribute Thickness Select the fleshing on/off button to turn-off geometric property visualisation. Material Properties Within LUSAS the specific heat is defined as a massless quantity. In order to calculate this quantity, the standard specific heat capacity for a material is multiplied by the density. The result is a material parameter in the correct massless units, in this case J m-3 C-1. The materials in this example have properties of steel. Attributes Material Isotropic… • On the Isotropic dialog enter the thermal conductivity as 60 > • Enter the specific heat as 3.7596E6 • Enter the attribute name as Steel (J,m,C) and click the OK button. • Assign the material attribute Steel (J,m,C) to the surfaces. Boundary Conditions Unsupported nodes in thermal analyses are assumed to be perfect insulators. The environmental conditions are defined using environmental loading. This loading defines the amount of convection to the environment that occurs. Attributes Loading… • Select the Environmental Temperature option and click Next • On the Environmental Temperature dialog enter the environmental temperature as 25 • Enter the convective heat transfer coefficient as 500 • Since radiation is to be ignored set 197 Thermal Analysis of a Pipe the radiation heat transfer coefficient to 0 • Enter the attribute name as Environmental Temperature and click the Finish button. • Select the 4 lines defining the outside of the pipe and assign the attribute Environmental Temperature to the these lines Ensure the option to Assign to lines is selected. Ensure Loadcase 1 and a Load factor of 1 are selected. Click OK to finish the assignment. The pipe is heated by the oil passing along inside the pipe. This is modelled using a prescribed heat input assigned to the lines defining the inner surface of the pipe. Attributes Loading… • Select the Prescribed Temperature option and click Next • On the Prescribed Temperature dialog enter a temperature of 150 • Ensure that the Total Prescribed temperature loading option is selected. • Enter an attribute name of Oil Temperature and click the Finish button. • Select the 4 lines defining the inner surface of the pipe and assign the attribute Oil Temperature to the these lines. Ensure the option to Assign to lines is selected and Loadcase 1 is chosen with a Load factor of 1. Click OK to finish the assignment Saving the model File Save Save the model file. Running the Analysis File LUSAS Datafile... A LUSAS data file name of Pipe will be automatically entered in the File 198 Running the Analysis name field. • Ensure that the options Solve now and Load results are selected. • Click the Save button to solve the problem. A LUSAS Datafile will be created from the model information. The LUSAS Solver uses this datafile to perform the analysis. If the analysis is successful... The LUSAS results file will be added to Treeview. In addition, 2 files will be created in the directory where the model file resides: Pipe.out this output file contains details of model data, assigned attributes and selected statistics of the analysis. Pipe.mys this is the LUSAS results file which is loaded automatically into the Treeview to allow results processing to take place. If the analysis fails... If the analysis fails, information relating to the nature of the error encountered can be written to an output file in addition to the text output window. Any errors listed in the text output window should be corrected in LUSAS Modeller before saving the model and re-running the analysis. Rebuilding a Model If it proves impossible for you to correct the errors reported a file is provided to enable you to re-create the model from scratch and run an analysis successfully. Pipe_modelling.vbs carries out the modelling of the example. File New… Start a new model file. If an existing model is open Modeller will prompt for unsaved data to be saved before opening the new file. • Enter the file name as pipe • Change the user interface to Thermal File Script Run Script... > To recreate the model, select the file pipe_modelling.vbs located in the \\Examples\Modeller directory. 199 Thermal Analysis of a Pipe File LUSAS Datafile... Rerun the analysis to generate the results Viewing the Results If the analysis was run from within LUSAS Modeller the results will be loaded on top of the current model and the loadcase results for loadcase 1 will be set active in the Treeview. • Remove the Geometry layer from the Treeview. • If necessary any visualised thermal loadings can be removed by deselecting Visualise Assignments from both thermal loading datasets in the Treeview. Temperature Contours With no features selected, click the right-hand mouse button in a blank part of the Graphics window and select the Contours option to add the Contours layer to the Treeview. The contour plot properties will be displayed. • Select Potential contour results component PHI • Click the OK button. From the analysis it can be seen that the maximum temperature the outer surface of the pipe reaches is 108.5 o C. This completes the steady state part of the example. 200 Transient Thermal Analysis Transient Thermal Analysis This part of the example extends the previously defined pipe model used for the steady state analysis. A file is supplied that can be used to recreate the model if required. If you are continuing from the first part of the example you have the option to save your model file as pipe_transient.mdl and continue from the heading ‘Setting up the Starting Conditions’. Creating a new model (if required) File New… Start a new model file. If an existing model is open Modeller will prompt for unsaved data to be saved before opening the new file. • Enter the file name as pipe_transient File Script Run Script... > • To create the model, import the file pipe_modelling.vbs located in the \\Examples\Modeller directory. Setting up the Starting Conditions The first step of a transient analysis is used to establish the steady state conditions before any heat is input. In this example this means the oil temperature needs to be removed from the first loadcase to allow the pipe to reach the environmental temperature before the oil temperature is introduced and the transient analysis begins. • Ensure the Geometry, Mesh and Attributes layers are present in the Treeview Treeview click the right-hand mouse button on the Oil Temperature • In the attribute and choose the Deassign> From all option. Now we define how the transient analysis should take place: • Using the right-hand mouse button click on Loadcase 1 in the select Nonlinear & Transient from the Controls menu. 201 Treeview and Thermal Analysis of a Pipe • Select the Time domain option. • Ensure Thermal is selected in the drop down list. • Enter an Initial time step of 0.001 • Leave the Total response time set to 100E6 • In the Common to all section, enter the Max time steps or increments as 1 • Click the OK button. Setting up the Transient Analysis Once the starting conditions have been established the transient analysis can begin. The heat input is assigned to the inner surface of the pipe and the time stepping regime is defined. Firstly reapply the environment temperature, which represents the atmospheric temperature. Treeview click on the attribute Environmental Temperature with the • In the right-hand mouse button and choose the Select Assignments option. This will select the lines using this attribute. 202 Transient Thermal Analysis • Drag and drop the attribute Environmental Temperature onto the graphics window to assign the attribute to Loadcase 2 by editing the loadcase name in the drop down list. Enter a Load factor of 1 and click the OK button. This will Treeview. introduce Loadcase 2 into the Now apply the Oil Temperature. • Select the lines defining the inner surface of the pipe. • Assign the dataset Oil Temperature to these Lines selecting Loadcase 2 with a factor of 1. Click OK to finish the assignment. • Using the right-hand mouse button click on Loadcase 2 in the select Nonlinear & Transient from the Controls menu. Treeview and • Select the Time domain option. • Ensure Thermal is selected in the drop down list. • Enter an Initial time step of 10 • In the Common to all section enter the Max time steps or increments as 120 203 Thermal Analysis of a Pipe • Click the OK button. Saving the model File Save Save the model file. Running the Analysis File LUSAS Datafile... A LUSAS data file name of pipe_transient will be automatically entered in the File name field. • Ensure that the options Solve now and Load results are selected. • Click the Save button to solve the problem. A LUSAS Datafile will be created from the model information. The LUSAS Solver uses this datafile to perform the analysis. Viewing the Results If the analysis was run from within LUSAS Modeller the results will be loaded on top of the current model and the loadcase results can be seen in the Treeview. To establish the time taken to reach the steady state condition a graph of external temperature verse response time is to be generated. • Select the node on the outside of the pipe as shown. Utilities Graph Wizard... • Choose the Time history option and click on the Next button Firstly we define the X axis data. • Select the Named and with Loadcases, All option selected click the Next button. • Choose Response Time from the drop down list and click the Next button. Then we define the Y axis data • Select the Nodal option and click the Next button. 204 Select this Node Viewing the Results • Select Entity Potential component PHI • Select Specified single node from the Extent drop down list and the selected node number will appear in the Selected Node drop down list. • Click the Next button. It is not necessary to input the graph titles at this stage. They can always be modified later. • Deselect the Show symbols option. • Click on the Finish button to display the graph showing the variation of temperature on the outer surface of the pipe with time. In can be seen that the outside of the pipe reaches its steady state condition after approximately 300 seconds. This completes the transient thermal example. 205 Thermal Analysis of a Pipe 206 Description Linear Analysis of a Composite Strip For software product(s): With product option(s): LUSAS Composite None. Description A 50mm x 10mm x 1mm thick composite strip, composed of an 8-layer composite material is to be analysed first using shell elements and then using solid elements in order to compare the results obtained. Distributed Loading This quarter only to be modelled 15 15 Simply supported The strip is loaded with 10 5 All Dimensions in mm a global distributed line load of 10N/mm on the centreline as shown. The composite strip has two axes of symmetry therefore only a quarter of the strip needs to be modelled. Symmetry boundary conditions are to be simulated by applying supports on the appropriate Lines. The geometry of the strip and support positions are as shown. 5 Units used are N, mm, t, s, C throughout. Analysis 1 Surface features meshed with thick shell composite elements. Analysis 2 Volume features meshed with solid composite elements 207 Linear Analysis of a Composite Strip Objectives The output from the shell analysis will consist of: Deformed Mesh Plot showing displacements with peak values annotated. Bending Stress Contour Plot showing the direct stresses on the bottom Surface. The output from the solid analysis will consist of: Deformed Mesh Plot showing displacements with peak values annotated. Bending Stress Contour Plot showing the direct stress on the bottom Surface of layer 1. Shear Stress Contour Plot showing the interlamina shear stress on the top Surface of layer 1. Keywords 2D, 3D, Composite, Shell, Solid, Lay-up. Interlamina Shear, Failure Criteria, Tsai-Wu Associated Files strip_shell_modelling.vbs carries out the modelling of the example using shell elements. strip_solid_modelling.vbs carries out the modelling of the example using solid elements. Modelling : Shell Model Running LUSAS Modeller For details of how to run LUSAS Modeller see the heading Running LUSAS Modeller in the Examples Manual Introduction. Note. This example is written assuming a new LUSAS Modeller session has been started. If continuing from an existing Modeller session select the menu command File>New to start a new model file. Modeller will prompt for any unsaved data and display the New Model dialog. 208 Modelling : Shell Model Creating a new model • Enter the file name as strip_shell • Use the Default working folder. • Enter the title as Composite Strip Shell Model • Set the units N,mm,t,s,C to • Select the startup template Composite from those available in the drop down list. • Select the Composite User interface • Select the Vertical Z axis option and click the OK button. Note. Selecting the startup template Composite will add useful composite specific modelling data to the Treeview. Note. Save the model regularly as the example progresses. Use the Undo button to correct any mistakes made since the last save was done. Defining the Geometry Geometry Surface Coordinates... > Enter coordinates of (0,0), (10,0), (10,5) and (0,5) and click OK to define the first Surface. • Select the Line on the right hand side as shown. Geometry Surface > By Sweeping… Enter a translation distance of 15 in the X direction. • Click the OK button to create a new Surface. 209 Select this Line Linear Analysis of a Composite Strip Meshing The Surfaces are to be meshed using thick shell elements. LUSAS provides a composite surface mesh attribute by default. This can be seen in the Treeview. A thick shell element (QTS4) is used. • Select the whole model. (Using the Ctrl and A keys together). • Drag and drop the surface mesh attribute Composite Shell from the onto the selected features. Treeview Modeller will draw a mesh based upon a default of 4 Line divisions per Line. This mesh density will be altered by using Line mesh datasets. Note. A number of Line mesh attribute are provided by LUSAS by default. These can simply be dragged and dropped onto the features to which they are to be assigned. With the whole model selected: • Drag and drop the Line mesh attribute Divisions=2 from Treeview the onto the selected features. Select all Lines for Line mesh 'Divisions=2' Select these 2 Lines for Line mesk 'Divisions=3' • Select the 2 horizontal Lines on the right-hand side of the model. (Hold the Shift key down to add to the initial line selection). Treeview onto • Drag and drop the Line mesh attribute Divisions=3 from the the selected features. This overwrites the previous Line mesh assignment. Checking Local Element Directions In creating the second Surface from the first the orientation of the Surface axes will not necessarily be the same. In this example the local element directions should be checked because the composite lay-ups which are defined later in this example are assigned to the model using the local element axes. 210 Modelling : Shell Model Use the isometric rotation button to rotate the model to a similar view to that shown. Note. If manually rotating the model pressing the Ctrl key at the same time will rotate the model in the plane of the screen. Treeview • In the double click Mesh and select the Show element axes option. • Click the OK button to display the element axes. The element axes in the right-hand section of the model need to be re-oriented to lie along the global X axis. Changing the Element Directions • Select the right-hand Surface of the model. Geometry Surface Cycle… > The orientation of the elements needs to be rotated to align them with the global X axis. • Geometry Surface Reverse > Click Apply to rotate the axis by 90 degrees each time, until the x axis match with those of the left-hand surface. The orientation of the elements will rotate to align the with the global Y axis. 211 Linear Analysis of a Composite Strip • In the Treeview double click the Mesh layer. The mesh properties dialog will appear. Show • De-select the element axes option and click the OK button. Defining the Geometric Properties The strip is 1mm thick. A geometric property attribute of unity thickness is provided by default. This can be used to define the thickness of the Surfaces. • Select the whole model and drag and drop the geometry attribute Unit Thickness from the Treeview onto the selected features. If the fleshing option is turned on the assigned geometric property will be automatically visualised. Select the fleshing on/off button to turn-off geometric property visualisation. Note. Once assigned to the model, attributes such as geometric assignments may be visualised. • In the Treeview click the right-hand mouse button on the geometry attribute Unit Thickness. Select Visualise Assignments to show where the attribute has been assigned to the model. • Follow a similar process and deselect Visualise Assignments to hide the attribute display again. Defining the Composite Material Properties The material properties of the strip will be modelled as a composite lay-up made up from 8 lamina each defined as an orthotropic material. Whilst LUSAS provides a range of material types by default this example is based upon a test study and requires specific material data to be defined. 212 Modelling : Shell Model Attributes Material Orthotropic… > To define the orthotropic material: • With the Elastic tab displayed, select a Solid model from the drop down list. • Enter the Young's Modulus in the X direction as 1E5, in Y as 5000 and in Z as 5000 • Enter the shear modulus in the XY plane as 3000, and in YZ and ZX as 2000 • Finally, enter Poisson's ratio as 0.4 in the XY plane, and 0.3 in the other two planes. It is not necessary to enter the mass density. • Enter the attribute name as Strip Material and click the OK button to add the material attribute to the Treeview. This will be assigned to the model later in the example. 213 Linear Analysis of a Composite Strip Defining the Composite Lay-up Arrangement Details of the composite stack are shown in the attached table. The stack is symmetrical about the mid plane. This enables the input of the stack to be reduced by using the symmetric option. Attributes Composite… • Select the Solids and Shells option and click Next • Ensure that the Normal tab is displayed for shells and solids. • Select the New button to enter the composite lay-up details. 214 Lamina Name Thickness Angle Lamina1 0.1 0 Lamina2 0.1 90 Lamina3 0.1 0 Lamina4 0.2 90 Modelling : Shell Model The Add Lamina dialog will appear. The Name for the first lamina will be automatically entered as Lamina1 The material will automatically be entered as Strip material • Change the lamina thickness to 0.1 • Enter the angle as 0 • Click the Apply button to define the lamina. Enter lamina 2, 3 and 4 in a similar manner using the values in the previous table. Click Apply after each lamina is defined. Note layer 4 has a different thickness to the other layers. Click OK when all are defined. • On the Solids and Shells dialog select the Symmetric option. • Enter the composite attribute name as Strip Layup Now check the composite input • On the Composite Materials dialog, select the Grid tab. • Ensure that the values are as shown. Visualising the Composite Lay-up arrangement • On the Solids and Shells dialog, select Visualise to view the lay-up sequence. 215 Linear Analysis of a Composite Strip • Click the Close button to return to the Composite Materials dialog. • Click the Finish button to add the composite material attribute to the Treeview. Note. The lay-up sequence always builds from the bottom to the top. In this example, Lamina1 is the bottom lamina in the stack. Note. Composite lay-up data may also be defined in external spreadsheets for copying and pasting into the composite layup Grid using the standard copy (Ctrl + C) and paste (Ctrl + V) keys. Assigning the Composite Lay-up Arrangement • To assign the composite attribute to the model, drag a box around the model to select all the features. • Drag and drop the attribute Strip Lay-up from the features. • On the Assign Composite dialog, ensure that Assign to Surfaces and that Local Element Axes are selected. • Click the OK button. Note. In a composite analysis, assigning the composite material lay-up automatically assigns the material attribute to the model at the same time. The composite material attribute therefore does not have to be directly assigned to features. 216 Treeview onto the selected Modelling : Shell Model Checking the composite orientation To check the orientation of each composite lamina is correct. Treeview and double click on the Attributes entry to display the • Select the attribute layer properties. • Select the Composite tab and select the Strip Layup option from the list. • Click on the Settings button and select the option to Visualise ply directions. • Click OK and OK again. • In the Treeview expand the Composite Strip layup entry and right-click on the lamina you wish to check and Set Lamina Active • When you are satisfied the orientations are correct deselect this visualisation by selecting the Treeview, double clicking on the Attributes entry, selecting the Composite tab and deselecting the Strip Layup option. Supports LUSAS provides the more common types of support by default. These can be seen in the Treeview. The model will be supported in the Z direction at the internal Line between the two Surfaces. 217 Linear Analysis of a Composite Strip • Select the internal Line shown Select this Line for 'Fixed in Z' support • Drag and drop the support attribute Fixed in Z from the Treeview onto the selected feature, click OK ensuring that it is assigned to All loadcases The supports visualised. will be Defining Symmetry Support Conditions LUSAS provides symmetry boundary conditions by default. These can be seen in the Treeview. As only a quarter of the structure has been modelled the symmetry boundary conditions are assigned to two sides of the model. • Select the 2 upper Lines of the model as shown Select these 2 Lines for support 'Symmetry XZ Plane' • Drag and drop the support attribute Symmetry XZ from the Treeview onto the selected features. • Click OK visualise supports. Select this Line for support 'Symmetry YZ Plane' to the • Select the right-hand Line of the model as shown. • Drag and drop the support attribute Symmetry YZ from the the selected Line. • Click OK to visualise the supports. 218 Treeview onto Modelling : Shell Model Loading The model will be subjected to a load per unit length of 5 N/mm acting in the negative Z direction along the right-hand line which represents the mid-span centre-line of the strip. Note. The composite strip is modelled using a quarter model and the Line of load application coincides with one of the Lines of symmetry. The value of applied load is therefore half of that applied to the full model. Attributes Loading… • Select the Global Distributed option and click Next • On the Global Distributed dialog select the Per Unit Length option. • Enter a value of -5 in the Z direction. • Enter the attribute name as Global Distributed • Click the Finish button to add the loading attribute to the Treeview. • Select the Line on the right of the model as shown. • Drag and drop the loading attribute Global Distributed from the Treeview onto the selected Line. Select this Line • Click the OK button to assign the load to the selected Lines and to accept the default loadcase. The loading will be visualised. Saving the model The model is now complete and the model data must be saved. File Save Save the model file. 219 Linear Analysis of a Composite Strip Running the Analysis With the model loaded: File LUSAS Datafile... A LUSAS data file name of strip_shell will be automatically entered in the File name field. • Ensure the Solve now and Load results options are selected. • Click the Save button to finish. A LUSAS Datafile will be created from the model information. The LUSAS Solver uses this datafile to perform the analysis. If the analysis is successful... The LUSAS results file will be added to Treeview. In addition, 2 files will be created in the directory where the model file resides: strip_shell.out this output file contains details of model data, assigned attributes and selected statistics of the analysis. strip_shell.mys this is the LUSAS results file which is loaded automatically into the Treeview to allow results processing to take place. If the analysis fails... If the analysis fails, information relating to the nature of the error encountered can be written to an output file in addition to the text output window. Any errors listed in the text output window should be corrected in LUSAS Modeller before saving the model and re-running the analysis. Rebuilding a Model If it proves impossible for you to correct the errors reported a file is provided to enable you to re-create the model from scratch and run an analysis successfully. strip_shell_modelling.vbs carries out the modelling of the example. File New… Start a new model file. If an existing model is open Modeller will prompt for unsaved data to be saved before opening the new file. • Enter the file name as strip_shell 220 Viewing the Results File Script Run Script... File LUSAS Datafile... > To recreate the model, select the file strip_shell_modelling.vbs located in the \\Examples\Modeller directory. Rerun the analysis to generate the results Viewing the Results If necessary, use the isometric rotation button to rotate the model to a similar view to that shown. Plotting peak vertical displacements • Select the display. Treeview and delete the Attributes and Geometry layers from the • With no features selected click the right-hand mouse button in a blank part of the Graphics window and select Values to add the Values layer to the Treeview. The values properties dialog will be displayed. • With the Value Results tab selected, select entity results for Displacement of component DZ. (Displacement in the Z direction). • Select the Values Display tab, de-select Maxima and specify that 0 % of the Minima displacement values are to be plotted 221 Linear Analysis of a Composite Strip • Click the OK button to display peak values of vertical displacement. • Delete the Values layer from the Treeview. Stress contour plots for lamina Note. For shell models the lamina results are output for the middle of each lamina selected. • Click the right-hand mouse button in a blank part of the graphics window and select Contours to add the contours layer to the Treeview. The Contour Properties dialog will be displayed. • Select the Stress - Thick Shell lamina entity of stress Sx Note. By default, the stresses will be calculated in the lamina material direction. The Transform button on the Contour Properties dialog can be used to transform stresses into global or user defined directions. • Click the OK button to display contours and the associated contour key. • Right-click on Lamina1 in the Treeview and Set Lamina Active. The contour key should be showing a maximum value of 519.2 • To display the mesh on top of the contours select the Mesh entry in the Treeview and drag on drop it on top of the Contour entry in the Treeview. • By selecting different lamina from the Composite Strip layup entry in the Treeview, the stresses throughout the composite strip can investigated. Note. Because there are discontinuities between laminae the stress plots produced will always be for un-averaged results. 222 Modelling : Solid Model Interlamina shear plots • In the Treeview double-click the Contours layer to display the contour layer properties. • Select the Stress - Thick Shell lamina entity of stress Szx • Click the OK button to display contours and the associated contour key for the active lamina. Modelling : Solid Model The composite strip in this example is now to be modelled using solid composite brick elements meshed onto Volumes. This is to compare the accuracy of the results obtained for each modelling method. Files. The shell composite model created in the first part of this example can be extended to create the solid composite model. To continue directly from the shell model toggle the menu entry Utilities>Mesh>Mesh Lock to ensure the Mesh Lock option is deselected and click Yes to confirm the closing of the results files. • Enter the model file name as strip_solid and click the Save button. File Save As... • Remove all layers from the Treeview. • Add the Geometry, Attributes and Mesh layers to the default properties by clicking OK on each dialog. Treeview. Accept all Rebuilding model from supplied file File New… Alternatively, start a new model file. If an existing model is open Modeller will prompt for unsaved data to be saved before opening the new file. • Enter the file name as strip_solid File Script Run Script... > To recreate the model, import the file strip_shell_modelling.vbs located in the \\Examples\Modeller directory. 223 Linear Analysis of a Composite Strip Changing the model description File Model Properties… • Change the model description to Composite strip - solid model and click OK Converting the Model from Shells to Solids To convert the 2D model that uses Surfaces into a 3D model that uses Volumes a number of attributes assigned to the 2D model need to be deassigned. This is to prevent them being copied when the Surfaces are swept to create a 3D model. Note. In the following tasks, take care to deassign and NOT delete the Loading, Support attribute, Composite strip lay-up attribute or the Geometric material attribute Treeview. from the Deassigning the loading • In the Treeview click the right-hand mouse button on the loading attribute Global Distributed and select Deassign>From all Deassigning the supports • In the Treeview, click the right-hand mouse button on the support attribute Fixed in Z, and select Deassign>From all • In the Treeview, click the right-hand mouse button on the support attribute Symmetry XZ, and select Deassign>From all. • In the Treeview, click the right-hand mouse button on the support attribute Symmetry YZ, and select Deassign>From all. Deassigning the composite material arrangement • Using the method described previously, deassign the composite attribute Strip Layup from the model. Deassign the geometry • Using the method described previously, deassign the geometry attribute Unit Thickness from all Surfaces on the model. Deassigning the Surface mesh • Using the method described previously, deassign the surface mesh attribute Composite Shell from the model. 224 Modelling : Solid Model Note. When the an attribute is de-assigned from the model such that it is not used on any feature the assigned attribute symbol will change from its coloured form to its unassigned grey form . In the Treeview the only assigned attribute left after this de-assignment process should be the 2 and 3 line mesh divisions and the strip material. Default mesh divisions The Lines on the model have been assigned different Line mesh divisions earlier in the example. However, the default number of line mesh divisions is still set by default to be 4. If the existing surfaces were swept to create volumes any newly created lines between the top and bottom surfaces would have the default of 4 mesh divisions per line assigned to them when in fact only one mesh division per line is required. To adjust the default number of mesh divisions • Select the Meshing tab. Set the default number of divisions to be 1 and click OK File Model Properties… Modifying the Geometry The 2D model will now be swept into 3D by sweeping the existing two Surfaces to create two Volumes. • Select the whole model. Geometry Volume By Sweeping... > Enter a translation in the Z direction of 1 and click OK If necessary use the isometric rotation button to rotate the model as shown. Note. With Composite analysis models the thickness of the volume defines the thickness of the strip and no geometric property thickness is required to be assigned to the model. The combined thickness of the composite material layups should equal the thickness of the volume. Meshing A Volume mesh is to be defined. LUSAS provides a number of volume mesh attribute by default. These can be seen in the Treeview. The composite brick element to be used has a hexahedral element shape and a quadratic interpolation order. 225 Linear Analysis of a Composite Strip • Select the whole model • Drag and drop the Volume mesh attribute Composite Brick (HX16L) Treeview onto the from the selected features. Note. The Line mesh divisions (defined in the shell model of this example) are used to create the mesh arrangement for the top and bottom Surfaces. The default number of Line mesh divisions are used for each swept Line on the side Surfaces. Assigning Composite Properties • With the whole model selected, drag and drop the Composite material attribute Strip Lay-up from the Treeview onto the selected features ensuring that it is assigned to Volumes using Local element axes. Click OK to carry out the assignment. Loading • Select the upper Line shown right. Select this upper Line • Drag and drop the loading attribute Global Distributed from the Treeview onto the selected feature and click OK Supports • Select the lower internal line as shown. Treeview onto the • Drag and drop the support attribute Fixed in Z from the selected feature, Click OK ensuring that Assign to lines is selected for All loadcases Select this lower Line 226 Running the Analysis In order to model the boundary conditions the supports must be assigned to the Surfaces that are, in effect, axes of symmetry for the entire strip. These supports are easier to assign on a view along the global Z axis. Set the view direction along the global Z axis by pressing the Z axis button on the status bar at the bottom of the graphics window. • Drag a box around Select these 2 Surfaces the 2 upper Surfaces of the model and drag and drop the support attribute Symmetry XZ from Treeview the onto the selected features, Click OK ensuring that Assign to surfaces is selected for All loadcases • Drag a box around the right-hand Surface of the model and drag and drop the support attribute Symmetry YZ from Treeview the Select this Surface onto the selected features, Click OK ensuring that Assign to surfaces is selected for All loadcases To view the applied supports use the isometric rotation button. Save the model The model is now complete. File Save Save the model file. Running the Analysis With the model loaded: 227 Linear Analysis of a Composite Strip File LUSAS Datafile... A LUSAS data file name of strip_solid will be automatically entered in the File name field. • Ensure the Solve now and Load results options are selected. • Click the Save button to finish. A LUSAS Datafile will be created from the model information. The LUSAS Solver uses this datafile to perform the analysis. If the analysis is successful... The LUSAS results file will be added to Treeview. In addition, 2 files will be created in the directory where the model file resides: strip_solid.out this output file contains details of model data, assigned attributes and selected statistics of the analysis. strip_solid.mys this is the LUSAS results file which is loaded automatically into the Treeview to allow results processing to take place. If the analysis fails... Use a text editor to view the output file and search for ‘ERROR’. Any errors listed in the output file should be fixed in LUSAS Modeller before saving the model and rerunning the analysis. Rebuilding the Model If errors are listed that for some reason you cannot correct, a file is provided to recreate the model information correctly, allowing a subsequent analysis to be run successfully. strip_solid_modelling.vbs carries out the modelling of the example. File New… Start a new model file. If an existing model is open Modeller will prompt for unsaved data to be saved before opening the new file. • Enter the file name as strip_solid File Script Run Script... File LUSAS Datafile... > To recreate the model, select the file strip_solid_modelling.vbs located in the \\Examples\Modeller directory. Rerun the analysis to generate the results 228 Viewing the Results Viewing the Results • If present, delete the Annotation and Contours layers from the Treeview If necessary, use the isometric rotation button to rotate the model as shown. Plotting peak vertical displacements • With no features selected click the right-hand mouse button in a blank part of the graphics window and select Values to add the values layer to the Treeview. The values properties dialog will be displayed. • With the Value Results tab selected, select Displacement results of displacement in the Z direction, DZ • Select the Values Display tab, de-select Maxima and specify that 0 % of the Minima displacement values are to be plotted. • Click the OK button to display the peak values of vertical displacement. • Delete the Values layer from the Treeview. 229 Linear Analysis of a Composite Strip Stress contour plots for lamina Note. For solid models the lamina results can be selected for the top, middle or the bottom of any selected lamina. • With no features selected click the right-hand mouse button in a blank part of the graphics window and select Contours to add the contours layer to the Treeview. The contour Properties dialog will be displayed. • Select entity results of Stress - Solids lamina (bottom) of component Sx and click the OK button. • In the Treeview expand the Composite Strip layup entry and right-click on the Lamina1 and Set Lamina Active The contour key should be showing a maximum stress in the lamina X direction of 679.4 • By re-ordering the layers in the Treeview the mesh can be viewed on top of the contour results. Interlamina shear plots • In the Treeview double-click the Contours layer to display the contour layer properties. 230 Viewing the Results • Select Stress - Solids lamina (top) contour results of stress Szx • Click the OK button to update the contours and the contour key to show the minimum value of -6.944 Defining Failure Strength Composite Composite Failure… The failure strength dialog will appear. • Enter the Dataset title as Layer Strength • Enter the Longitudinal Tensile Strength as 1978 • Enter the Transverse Tensile Strength as 48.69 • Enter the Compressive 1978 Longitudinal Strength as • Enter the Transverse Compressive Strength as 48.69 • Enter the Shear Strength as 133 • Leave the interaction type as Default and click OK Assigning Failure Strength The failure strength is assigned to the geometry. • Select the whole model. 231 Linear Analysis of a Composite Strip • From the Treeview drag and drop Layer Strength onto the selected features and click OK to Assign to volumes Plotting contours of Failure Criteria • In the Treeview double-click the Contours layer. • Select Stress - Solids lamina (bottom) contour results of Tsai-Wu failure, T-Wu. By default, the stresses will be shown in the laminate material direction. • Select the Contour Display tab and pick the Contour Key Details button, change the number of significant figures to 2 and deselect the Show minimum value option. • Click OK to update the contour key details and OK again to display contours of the Tsai Wu failure criteria. Note. Values greater than unity show that the material has exceeded the failure criteria. In this example the maximum failure value (shown on the contour key) is only 0.28 so no failure has occurred due to the applied loading. This completes the example. 232 Description Damage Analysis of a Composite Plate For software product(s): With product option(s): LUSAS Composite plus Nonlinear. Description A composite plate 70 mm made up from an IM Carbon cross ply laminate is placed under tensile loading to analyse the 30 mm damage growth and 10 mm Diameter stress redistribution around a stress concentration caused by a 10mm diameter hole. Because of symmetry a quarter model will be created. Units used are N, mm, t, s, C throughout. Objectives The objective of the analysis is: To determine the onset of damage growth To predict the effect of damage growth on the stress distribution within the composite stack Keywords Composite, Hashin, Damage, Nonlinear 233 Damage Analysis of a Composite Plate Associated Files composite_plate_modelling.vbs carries out the modelling of the example. Modelling Running LUSAS Modeller For details of how to run LUSAS Modeller see the heading Running LUSAS Modeller in the Examples Manual Introduction. Note. This example is written assuming a new LUSAS Modeller session has been started. If continuing from an existing Modeller session select the menu command File>New to start a new model file. Modeller will prompt for any unsaved data and display the New Model dialog. Creating a new model • Enter the file name as composite_plate • Use the Default working folder. • Enter the title as Damage Analysis of Composite Plate • Set the units as N,mm,t,s,C • Select the startup template Composite • Select the User Interface Composite • Select the Vertical Z axis. • Click the OK button. Note. Save the model regularly as the example progresses. Use the Undo button to correct any mistakes made since the last save was done. Feature Geometry The composite plate will be modelled as a quarter model and symmetry boundary conditions will be used to reduce the size of the model. Firstly the hole will be defined. 234 Modelling Geometry Line > Arc/Circle > From Coords/Points... • Enter coordinates of (5, 0), (0, 5) and (0, 0) • Select the Centre option next to the (0, 0) coordinate entry and click the OK button. Now define the lines representing the edges of the specimen. Geometry Line Coordinates… > Enter coordinates of (35, 0), (35, 15) and (0,15) and click the OK button. Now create the lines on the symmetry planes. • Select the two points on the horizontal plane of symmetry Geometry Line Points… > Points on vertical plane of symmetry Points on horizontal plane of symmetry Create a line along the horizontal line of symmetry. • Select the two points on the vertical plane of symmetry. Geometry Line Points… > Create a line along the vertical line of symmetry. Now create a surface from the boundary lines. • Change the selection mode so only Lines are selected from the display. Click and hold the left-hand mouse button on the selection button , then click on the button to select only lines. • Box-select all the lines in the model by clicking and dragging the cursor around all the lines that form the surface. Geometry Surface Lines… > Create a surface from the selected lines. 235 Damage Analysis of a Composite Plate • Change the selection mode back to the default pointer Meshing In this example the mesh will be graded manually by specifying the number of elements on each of the boundary lines. Define a null line mesh with 16 divisions. Attributes Mesh Line… • Enter 16 in the number of divisions. > • Enter the dataset name as Divisions=16 and click the OK button. • Use the Ctrl and A keys together to select all the features and assign Divisions=16 from the Treeview to all lines. • Select the upper horizontal line representing the edge of the plate and assign the line mesh dataset Division=8 from the Treeview. This will overwrite the previous assignment. • Select the line on the right hand side of the model and assign Divisions=2 from the Treeview. This will overwrite the previous assignment. The surface will now be swept through the depth of the plate to create a volume. Lines on the newly created surface on the back face of the volume will automatically inherit the line mesh dataset from the swept surface. The lines through the depth will however adopt the default number of mesh divisions. Since one element only is required through the depth of the plate the default number of mesh divisions must be set to one. File Model Properties… • Select the Meshing tab. • Change the default number of mesh divisions to 1 and click OK Now the volume that represents a quarter of the plate can be created. • Select the Surface (use the Ctrl and A keys together to select whole model). Geometry Surface > By Sweeping… Sweep the surface to form a volume. • Enter a translation in the Z direction of 1 and click the OK button. Rotate the model to an isometric view to see the volume created. Now we assign a mesh to the volume. Because it is not a regular volume, a transition mesh is required. 236 Modelling • Double click on the mesh dataset Composite Brick (HX16L) and select the Allow transition pattern option. Note. Transition meshing is required to enable the five sided surface to be modelled predominantly with quadrilaterals. When using transitional meshing Modeller will introduce compatible triangular elements as necessary. • Click OK to change the mesh dataset. • Use the Ctrl and A keys to select the whole model and assign the mesh dataset Composite Brick (HX16L) to • Click on return the model to the default view from the Z axis. Material Properties Properties of a number of the more commonly used composite materials are available from the composite library. The plate in this example is made up from a four layer stack of IM Carbon UD. Attributes Material Composite Library… > • Select the material IM Carbon UD Vf=60% from the drop down list. • Leave the units set as N,mm,t,s,C • Ensure the option for 3D Solid is chosen and select the option to output parameters for the Hashin damage model • Click the OK button to add the selected composite material properties to the Treeview. 237 Damage Analysis of a Composite Plate Defining the Composite Stack • Select the Solids and Shells option and click Next • Select the New button Attributes Composite… The Add Lamina dialog will appear. The Name for the first lamina will be automatically entered as Lamina1 The material will automatically be entered as IM Carbon UD Vf=60% (Damage) (N,mm,t,s,C) • Leave the thickness as 1 and the angle as 0 • Click the OK button to define the lamina and return to the main dialog. • Select the New button again to define lamina 2 • Lamina2 will be automatically entered for the lamina name • Leave the thickness as 1 but change the angle to 90 • Ensure that material dataset IM Carbon UD Vf=60% (Damage) (N mm t s C) is selected. 238 Modelling • Click the OK button. • Select the Symmetric button to generate a four layer stack. • Enter the dataset name as Laminate Stack and click the Finish button. Assigning the Composite Stack The composite stack now needs to be assigned to the volume so that the zero fibre directions run along the length of the plate. To do this, a local coordinate system is defined such that the local axes defined correspond to the global axes. The composite stack is then assigned relative to this local coordinate system. Attributes Local Coordinates… • Ensure a Rotate Angle of 0 about the Z-axis is set. Enter the dataset name as Global and click the OK button. • Use Ctrl and A keys together to select the whole model and from the Treeview drag and drop the composite dataset Laminate Stack onto the selected features. • On the Assign Composite dialog ensure Assign to Volumes is selected. Select the Local Coordinate option, ensure the dataset Global appears in the drop down list and click the OK button. Visualising lamina directions Now the laminate stack is assigned to the model the lamina orientation can be checked by visualising the lamina directions. 239 Damage Analysis of a Composite Plate • In the Treeview click on Attributes with the right hand mouse button and select Properties • Select the Composite tab, then select the All datasets option. • Click on the Settings button. • On the Visualisation Settings dialog select the Visualise ply directions option and ensure Surface position Middle and Axis x are selected. • Click the OK button to return to the Attribute properties. • Click the OK button to visualise the layer directions. • In the Treeview, in the Composite Laminate Stack section right-click on lamina 1 and select the Set Lamina Active option. • Other lamina directions may be checked by setting each lamina active in turn. • Switch off visualisation of the layer directions by selecting Attributes in the mouse click. Treeview using a right hand • Select Properties, select the Composite tab choose the None option and click OK Supports Symmetry supports need to be assigned to the lines of symmetry of the model. 240 Modelling 1. Drag a box to select this vertical Surface and assign support Symmetry YZ Plane 3. Drag a box to select this vertical Surface and assign support Fixed in Z 2. Drag a box to select this vertical Surface and assign support Symmetry XZ Plane • Drag a box around the Surface on the vertical axis of symmetry. • Drag and drop the support dataset Symmetry YZ from the Treeview. • Ensure the Assign to surfaces option is selected and click OK to assign the support dataset. • Similarly drag a box around the Surface on the horizontal axis of symmetry and assign the support dataset Symmetry XZ from the Treeview to it. The model also needs to be restrained from moving in the out of plane direction. • Drag a box around the Surface on the right hand side of the model and assign the support dataset Fixed in Z from the Treeview. Loading The plate is to be placed under a tensile loading using a prescribed displacement. Attributes Loading… • Select the Prescribed Displacement option and click Next > • Enter a Total displacement of 0.1 in the X direction. • Enter a dataset name of Prescribed Displacement and click the Finish button. • Drag a box around the Surface defining the right hand end of the plate and assign the dataset Prescribed Displacement from the Treeview. • Click OK to assign to Loadcase 1 with a factor of 1 241 Damage Analysis of a Composite Plate Select the isometric view button and check the supports and loading have been applied as shown in this image. Analysis Control Because this is a nonlinear problem the load incrementation strategy needs to be defined. Treeview right-click on Loadcase 1 and from the Controls option • From the select the Nonlinear & Transient option. The Nonlinear & Transient dialog will appear. • Select the Nonlinear option. • Set Incrementation to Automatic • Set the Starting load factor to 0.5 • Set the Maximum change in load factor to 0.25 • Set the Maximum total load factor as 1 • Change the Incremental displacement norm to 100 as convergence is to be monitored on the residual norm only. • Leave the Maximum number of time steps or increments as 0 as this ensures the solution will continue until the maximum load is reached. 242 Running the Analysis • Click the OK button to finish. To avoid mechanisms in the element formulation when some of the Gauss integration points fail, it is necessary to switch on fine integration for the elements. File Model Properties… • Select the Solution tab and click on the Element Options button. Ensure that Fine integration for stiffness and mass is selected and click OK. Click OK to finish. Saving the model File Save Save the model file. Running the Analysis File LUSAS Datafile... A LUSAS data file name of composite_plate will be automatically entered in the File name field. • Ensure that the options Solve now and Load results are selected. 243 Damage Analysis of a Composite Plate • Click the Save button to solve the problem. Note. In running this nonlinear analysis a number of load increments are evaluated. An indication of the time remaining can be obtained by observing the number of the increment being evaluated. A LUSAS Datafile will be created from the model information. The LUSAS Solver uses this datafile to perform the analysis. If the analysis is successful... The LUSAS results file will be added to Treeview. In addition, 2 files will be created in the directory where the model file resides: composite_plate.out this output file contains details of model data, assigned attributes and selected statistics of the analysis. composite_plate.mys this is the LUSAS results file which is loaded automatically into the Treeview to allow results processing to take place. If the analysis fails... If the analysis fails, information relating to the nature of the error encountered can be written to an output file in addition to the text output window. Any errors listed in the text output window should be corrected in LUSAS Modeller before saving the model and re-running the analysis. Rebuilding a Model If it proves impossible for you to correct the errors reported a file is provided to enable you to re-create the model from scratch and run an analysis successfully. composite_plate_modelling.vbs carries out the modelling of the example. File New… Start a new model file. If an existing model is open Modeller will prompt for unsaved data to be saved before opening the new file. • Enter the file name as composite_plate and click OK File Script Run Script... File LUSAS Datafile... > To recreate the model, select the file composite_plate_modelling.vbs located in the \\Examples\Modeller directory. Rerun the analysis to generate the results 244 Viewing the Results Viewing the Results Loadcase results for each increment can be seen in the Treeview. If the analysis was run from within LUSAS Modeller the results will be loaded on top of the current model and the loadcase results for the first load increment are set active by default. If necessary, select the isometric view button. • If present, remove the Geometry and Attributes layers from the Treeview. Stress Contours • In the Treeview, right-click on the final load increment for Increment 3 Load Factor = 1 and select the Set Active option. For solid models the lamina results can be selected for the top, middle or the bottom of any selected lamina. For this results for the middle of selected laminae will be viewed. • With no features selected click the right-hand mouse button in a blank part of the graphics window and select Contours to add the contours layer to the Treeview. The contour Properties dialog will be displayed. • Select entity results of Stress - Solids lamina (middle) of component Sx and click the OK button. Treeview • In the expand the Composite Strip layup entry and right-click on the Lamina1 and Set Lamina Active The contour key should be showing a maximum stress in the lamina X direction of 3.16E3 • By re-ordering the layers in the the contour results. Treeview the mesh can be viewed on top of 245 Damage Analysis of a Composite Plate • In the Treeview, in the Composite Laminate Stack entry, right-click on Lamina2 and Set Lamina Active The contour key should be showing a maximum stress in the lamina X direction of 555.3 Note. When displaying layer contours the contours are displayed at the layer position through the thickness of the model. This completes the example. 246 Description Mixed-Mode Delamination For software product(s): With product option(s): LUSAS Composite Plus. Description This example demonstrates the use of delamination elements in a 2D analysis. Both 2D and 3D elements are available within LUSAS. These elements have the ability to model all modes of crack growth under mixed-mode conditions - mode I (open) mode II (shear) and mode III (tear 3D only). 30 mm Starter Crack P1=0.2125P 50 mm P2=0.7125P 3 mm 100mm Interface Properties Fracture Energy = 4 Initiation Energy = 57 HS Carbon UD Vf=60% The model is required to predict the growth of a crack within a unidirectional composite laminate subjected to mixed-mode loading. A starter crack 30 mm long is introduced at one end of a double cantilever beam (DCB) specimen. A tensile (crack opening) load is applied to the cracked end of the sample while a compressive (crack closing) load is applied to the centre of the specimen. The resulting delamination crack propagates along the length of the sample under mixed-mode conditions. The DCB specimen is constrained at either end and prescribed displacements are applied to the centre of the span in a negative Y direction and to the cracked arm, in a positive Y direction. No axes of symmetry other than the plane strain assumption may be made. The geometry of the strip and support positions are as shown. Units of N, mm, t, s, C are used throughout. 247 Mixed-Mode Delamination Objectives This analysis will: Predict the initiation of delamination Predict the propagation of a delamination crack with increasing displacement Produce an animated Deformed Mesh Plot showing the growth of delamination Produce a Contour Plot showing the redistribution of direct stress caused by delamination on the cracked Surface. Produce an animated Yield Plot showing the behaviour of the interface during incrementation Keywords Delamination, Composite, Shell, Nonlinear, Yield Symbol, Contour Plot, Animation Associated Files delamination_modelling.vbs carries out the complete modelling of the example. Modelling : Delamination Model Running LUSAS Modeller For details of how to run LUSAS Modeller see the heading Running LUSAS Modeller in the Examples Manual Introduction. Note. This example is written assuming a new LUSAS Modeller session has been started. If continuing from an existing Modeller session select the menu command File>New to start a new model file. Modeller will prompt for any unsaved data and display the New Model dialog. Creating a new model • Enter the file name as delamination • Use the Default working folder. • Enter the title as Delamination Model • Set the units to N,mm,t,s,C • Select the startup template Composite 248 Modelling : Delamination Model • Select the Composite User Interface. • Select the Vertical Y axis option. • Click the OK button. Note. Selecting the startup template Composite adds useful composite specific modelling data to the Treeview. Note. It is useful to save the model regularly as the example progresses. Use the Undo button to correct any mistakes made since the last save was done. • Select the Meshing tab and set the default number of divisions to 2 File Model Properties… • Select the Solution tab, select Element Options and select the option for Fine integration for stiffness and mass • Click the OK button to set the element options and the OK button to set the model properties. Defining the Geometry Geometry Point Coordinates... > Enter coordinates of (0,0), (30,0), (50,0) and (100,0) and click OK to define the Points. • Use the Ctrl and A keys together to select the Points just defined. Geometry Line Points... > Defines a series of straight Lines between the Points. • Select the whole model using the Ctrl + A keys together. Geometry Surface > By Sweeping… Ensure that the Translate option is selected and enter a value of 1.5 in the Y direction. • Click the OK button to finish to generate the first half of the model. The second half of the model will now be created by copying the existing data and specifying a suitable gap to enable the interface elements to be embedded in the model. Once the interface elements have been assigned this gap will be closed. • Select the whole model using the Ctrl + A keys. 249 Mixed-Mode Delamination Geometry Surface Copy… > Ensure that the Translate option is selected and enter a value of 20 in the Y direction. Note. At this stage the two halves of the model are separated to simplify the definition of the delamination interface elements. Meshing Delamination modelling requires a fine mesh density. The mesh density is controlled using Line mesh attributes. Attributes Mesh Surface… > • Select Plane strain, Quadrilateral, Quadratic elements. Ensure the Regular mesh option is selected with automatic divisions so that Modeller uses the default number of mesh divisions on each line. • Give the attribute the name Plane Strain Mesh • Click the OK button to add the attribute to the Treeview. • Select the whole model using the Ctrl + A keys. • Drag and drop the Plane Strain Mesh attribute from the selected features. Treeview onto the Treeview contains some commonly used line meshes. Null line meshes with The 10 and 30 divisions need to be added to those present. Attributes Mesh Line… > • With the Element description set to None define a line mesh attribute containing 10 divisions and named Divisions=10 • Click the Apply button to add the attribute to the Treeview. • Edit the number of divisions to 30 and change the attribute name to Divisions=30 • Click the OK button to add the attribute to the 1. Assign Divisions=10 to these Lines Treeview. 2. Assign Divisions=30 to these Lines 250 Modelling : Delamination Model • Assign the Divisions=10 attribute to the horizontal lines on the left-hand section of the model. • Assign the Divisions = 30 attribute to the remaining horizontal lines of the rest of the model to give a mesh arrangement as shown. Interface Elements Attributes Mesh Line… > • On the Line Mesh dialog define an Interface, 2-dimensional, Quadratic line mesh with 30 divisions. • Name the dataset Interface mesh • Click OK to add the dataset to the Treeview. • Select the two horizontal lines on the right-hand side of the upper face of the bottom set of surfaces as shown in the following diagram. 2. Select these lines 1. Select these lines and add to selection memory Edit Selection Memory > Set • Add these two lines to Selection Memory. These will form the slave surfaces of the interface elements. Note. Items can also be added to selection memory by using the right-hand mouse button in the display area and selecting the Selection Memory>Set menu entry from the popup menu. 251 Mixed-Mode Delamination Note. The order in which the lines are selected is important. The interface elements are drawn between sequential pairs of lines in the two selections, i.e. the first set will be drawn between the first line in the selection memory and the first line in the selection. • Select the two horizontal lines on the right-hand side of the lower face of the top set of surfaces as shown in the previous diagram. Ensure the surfaces in the selection match those in selection memory as described in the note above. • Drag and drop the Interface mesh attribute onto the model. Ensure Mesh from master to slave is selected. Click OK to finish the assignment. Edit Selection Memory > Clear • Clear the selection memory. Note. It is only necessary to make use of Selection Memory if assignment of the interface mesh is to be carried out on more than one line in one operation. By selecting a lower master line, holding the Shift key down, and selecting the corresponding upper slave line the assignment could also be carried out on a line by line basis. Composite Material LUSAS provides a number of the more common types of composite material in the Composite Material Library. In this example the component is fabricated from a unidirectional High Strength Carbon fibre reinforced polymer matrix composite. Attributes Material Composite Library… > • Select HS Carbon UD Vf=60% from the drop down box. • Set the units as N,mm,t,s,C • With the Composite properties option selected, choose Plane Strain and click the OK button to add the properties to the Treeview. 252 Modelling : Delamination Model The composite material is assigned to the surfaces of the model. Firstly check the surface axes to show the directions for the orthogonal material. Treeview click the right-hand mouse button on the Geometry layer and • In the select Properties • On the dialog select the Surface Axes option and click the OK button. All surfaces should appear with the double arrow (X direction) horizontal. • De-select the display of Surface axes as described above. Now assign the material properties: • Select the whole model using the Ctrl + A keys. • Select the HS Carbon UD Vf=60% Plane Strain (N,mm,t,s,C) attribute from the Treeview and drag and drop it onto the model. • Ensure the Assign to surfaces option is selected on the pop up dialog and click OK Interface Material Information concerning the fracture energies and the initiation stresses for the relevant failure modes are defined to describe the behaviour of the interface delamination model. For this example it is assumed that the interface characteristics are similar for the two modes. Mode 1 representing opening and mode 2 shear. Attributes Material > Specialised > Delamination Interface… • Ensure the number of fracture modes equals 2 (default) • Enter the value 4 for the fracture energy and 57 for the initiation stress for both modes. • Name the attribute Interface Material and click on OK to add the attribute to the Treeview. 253 Mixed-Mode Delamination Note. The interface material attribute need only be assigned to the master features. • Click the right-hand mouse button on the Interface Mesh attribute in the Treeview and choose the Select Master Assignments option from the drop down menu. • Drag and drop the Interface Material attribute from the model to assign to Lines. Treeview onto the Supports LUSAS provides the more common types of support by default. These can be seen in the Treeview. The model will be supported in the Y direction at the cracked (lefthand) end and in the X and Y directions at the uncracked (right-hand) end. 254 Modelling : Delamination Model • Select the point at the bottom left-hand corner of the model, drag and drop the support attribute Fixed in Y onto the selection and click OK to assign to Points. • Select the point at the bottom right-hand corner of the model, drag and drop the support attribute Fixed in XY onto the selection and click OK to assign to Points. The supports will be visualised as shown. Loading The model is subjected to two prescribed displacements. The left-hand (cracked) end of the model has a crack opening load assigned to it. A crack closing load is assigned to the mid-span. Attributes Loading… The structural Loading attributes dialog will be displayed. • With the Concentrated option selected click Next • On the Concentrated dialog enter a Concentrated load in Y Dir of 0.2125 • Enter the attribute name as Opening • Click the Apply button to add the attribute to the Treeview. • Edit the value in the Y direction to be -0.7125 • Enter the attribute name as Closing • Click the Finish button to add the loading attribute to the Treeview. Now assign the loads to the model. • Select the uppermost Point in the top left-hand corner of the model. • Drag and drop the loading attribute Opening from the selected Point. Treeview onto the • Click the OK button to accept the default Loadcase 1 with a Load factor of 1 and assign the loading to the model. 255 Mixed-Mode Delamination Select this Point to assign Opening load Select this Point to assign Closing load • Select the uppermost Point in the middle of the top section of the model. • Drag and drop the loading dataset Closing from the selected Point. Treeview onto the • Click the OK button to accept the default Loadcase 1 with a Load factor of 1 and assign the loading to the model. The loading will be visualised. Final Geometry Manipulation It is significantly easier to assign the appropriate mesh and the material properties of the interface region to the model if the interface surfaces are apart. Once these manipulations are complete it only remains to close the interface to complete the construction of the model. • Select the top section of the model. Drag a box to select the top section of the model 256 Modelling : Delamination Model Geometry Point > Make Unmergable Geometry Point Move... > Make the points of the upper section unmergable. This will ensure the nodes either side of the embedded crack in the model are not merged together. Note that making points unmergable will also ensure that the lines are also unmergable Move the selection to join the bottom half of the model by selecting the Translate option, enter a value of -18.5 in the Y direction and click OK to confirm. Analysis Control Since this is a nonlinear problem the load incrementation strategy needs to be defined. The analysis is to be terminated when the vertical displacement at the lefthand tip of the specimen reaches 6mm. • Select the point at the top-left of the model where the opening load is applied. Treeview click the right hand mouse button on Loadcase 1 and • From the select Nonlinear & Transient from the Controls menu. The Nonlinear & Transient dialog will be displayed. 257 Mixed-Mode Delamination • Select the Nonlinear option. • Set Incrementation to Automatic • Set the Starting load factor to 10. This will multiply the applied loading by a factor of 10 on the first load increment. • To enable the load to increase as required set the Max total load factor to 0 • To prevent the analysis carrying on too long if an error has been made set the maximum number of time step or increments to 50 • In the Incremental LUSAS file output section set the Plot file value to 3. This will ensure results are output to the Modeller plot file every third load increment. • In the Incrementation section on the top-left of the dialog select the Advanced button. • Select Use arc length control • Select the option to Use root with lowest residual norm 258 Modelling : Delamination Model • In the Termination criteria section select the Terminate on value of limiting variable option. The point at the top left-hand corner of the model should be entered in the drop down list. Note that this may not be the same point number as shown in this dialog. • Select the Variable type as V and the value as 6 • In the Step reduction section of the form ensure the Allow step reduction option is selected and set the Load reduction factor to 0.75 • Click the OK button to return to the control dialog. • Click the OK button to exit the Nonlinear & Transient dialog. Saving the model The model is now complete and the model data must be saved. File Save Save the model file. 259 Mixed-Mode Delamination Running the Analysis With the model loaded: File LUSAS Datafile... A LUSAS data file name of delamination will be automatically entered in the File name field. • Ensure Solve now and Load results are selected. • Click the Save button to finish. Note. In running this nonlinear analysis 33 load increments are evaluated. On modern personal computers this will take just a matter of minutes. An indication of the time remaining can be obtained by observing the number of the increment being evaluated. A LUSAS Datafile will be created from the model information. The LUSAS Solver uses this datafile to perform the analysis. If the analysis is successful... The LUSAS results file will be added to the Treeview. In addition, 2 files will be created in the directory where the model file resides: delamination.out this output file contains details of model data, assigned attributes and selected statistics of the analysis. delamination.mys this is the LUSAS results file which is loaded automatically into the Treeview to allow results processing to take place. If the analysis fails... If the analysis fails, information relating to the nature of the error encountered can be written to an output file in addition to the text output window. Any errors listed in the text output window should be corrected in LUSAS Modeller before saving the model and re-running the analysis. Rebuilding a Model If it proves impossible for you to correct the errors reported a file is provided to enable you to re-create the model from scratch and run an analysis successfully. delamination_modelling.vbs carries out the complete modelling of the example. 260 Viewing the Results File New… Start a new model file. If an existing model is open Modeller will prompt for unsaved data to be saved before opening the new file. • Enter the file name as delamination File Script Run Script... File LUSAS Datafile... > To recreate the model, select the file delamination_modelling.vbs located in the \\Examples\Modeller directory. Rerun the analysis to generate the results Viewing the Results Once the model has been successfully run and the results file loaded on top of the of the model file, an examination of the results can begin. The first stage in any results post-processing is to examine the deformed mesh. Plotting the deformed mesh The outline of the crack which has been initiated and grown during the solution with load incrementation may be observed using a solid representation of the model. For this the deformed mesh will be examined alone. All of the model information currently displayed must be removed. • Select each of the entries under the the graphics display. Treeview and delete them in turn to clear • With no features selected click the right-hand mouse button in a blank part of the graphics area and select Deformed Mesh • Select the Specify Factor option and give the value of 1 • Click on the Mesh tab. • Select the Solid and Outline only options. • Click the OK button to add the deformed mesh layer to the Treeview. Note. It is useful to use a magnification factor for displaying the deformed mesh for nonlinear analyses so that change in shape through the analyses can be observed. Treeview and make it active by • Select the last available loadcase from the clicking the right-hand mouse button and choosing the Set Active option. 261 Mixed-Mode Delamination The deformed mesh plot for the final loadcase increment will be displayed. Plotting the load deflection graph • Select the node at the top left-hand corner of the model where the opening load is applied. Utilities Graph Wizard… • With Time history selected click Next • With the Nodal option selected click Next • Select Entity Displacement with Component RSLT • The selected node will be visible in the drop down box. Click Next • Select the Named option and click Next • From the drop down list pick Total Load Factor and click Next • Enter the desired graph titles and click Finish to display the load deflection graph. • Close the graph window. 262 Viewing the Results Stress contours The growth of the delamination seen in the deformed mesh affects the stress distribution within the structure. This stress redistribution is easily visualised using stress contour plots. • With no features selected click the right-hand mouse button in a blank part of the Graphics area and select Contours to add the Contours layer to the Treeview. The Contour Properties dialog will be displayed. • Select Stress - Plane Strain contour results in the direction SX • Click the OK button to finish. The contour plot and the associated contour key will be displayed. Animating the effect of delamination growth By setting other loadcase attributes active the effect of the delamination growth on the stress distribution may be observed. The most effective way to view this effect is to animate the deformed mesh with the stress contours layer showing. Before animating each loadcase the contour range must be set to avoid the contour key changing between animation frames. • Double click on the Contours layer in the Treeview. • Select the Contour Display tab. • Deselect the Contour key option. • Select the Contour Range tab. • Select the Maximum and Minimum values and insert 1000 and -1000 • Select the Set as global range option • Click the OK button to finish. 263 Mixed-Mode Delamination Utilities Animation Wizard... To create the animation • Select Load History • Select Next • Select delamination.mys from the drop-down menu. • Select the All Loadcases check-box. • Select Finish to create an display the animated sequence. Note. Animations may be saved for replay using other Windows animation players using the File>Save As AVI menu option. After viewing the animation close the animation window and maximise the graphics window. Yield Plot The interface material formulation is an energy based model. The model allows the material to display three zones of behaviour. These are the elastic, softening and failed regions. Yield flags may be used to indicate which nodes within the model (if any) lie within a particular region. This technique allows a precise demonstration of the delamination crack extent within the model. • From the Treeview select and delete the Contours layer. • With no features selected, click the right hand mouse button in the graphics window and select the Values layer from the menu. • In the Properties dialogue box select the entity as Stress - Interface Elements and the component Yield • Click OK to display the softening zone. 264 Viewing the Results The extent of the delamination for the current loadcase can be clearly seen. The delamination growth can be visualised by animating this plot through successive loadcases. To create an animation of the delamination growth. Utilities Animation Wizard... • Select Load History • Select Next • Select delamination.mys from the drop-down menu. • Select the All Loadcases check-box. • Select Finish This completes the example. 265 Mixed-Mode Delamination 266